Hi, my name is Robert Feranec, and in this video, you are going to design a board in Cadence OrCAD and Allegro software. Even if you have never ever designed any board before, when you follow this tutorial step by step, then by the end of this video, you will design this board, and you will know how to use OrCAD and Allegro for your own projects. In this tutorial, you will learn how to draw schematic in OrCAD, you will learn how to create schematic symbols in schematic symbol library, so this will help you to create any symbol, which you may ever need in your schematic, you will learn how to create pads and footprints for all the components what you may need in your PCB, and of course, we are going to create the PCB in Cadence Allegro. So, you will learn how to place the components on the board and how to connect them together. We are going to also generate all the documents, which you need to manufacture this PCB, so for example you will know how to generate any Gerber files, you will also know how to generate all the kind of different documentation, for example assembly drawing and also BOM, bill of material, which you will need when you will be building your board. So, let's start. We are going to start OrCAD, click on Start button, find Cadence, Capture CIS, and select the license which you have. Left-click, OK. Click on File, New, Project, I'm going to call it LED_Youtube, and I'm going to save it here. Select folder, OK. I go inside of this DSN, Schematic, I'm going to rename schematic page, right-click, Rename, I'm going to call it LED, OK, and I'm going to rename also this, right-click, Rename, and I'm going to call it LED Project, OK. Select library, click on File, New, Library, right-click on the new library, Save as, be sure you are going to save it inside of our project directory, and I'm going to call it LED SchLib like this. Save. We are going to create our first schematic symbol, go to Google, search for DigiKey, and our first symbol is going to be header 2.54 millimeter. Click here, we would like to use Molex, here it is, in stock, with 3D model, Apply, and we need 2 positions, 1 row, board to cable/wire, through hole, Apply, let's have a look what they have here. We can use this one, so click here, and this is what we are going to use. Copy the header description, just left-click here, go back to OrCAD, and to create new component in your schematic symbol library, just right-click on the library, and use New Part, left-click. We are going to use the header description as the name, so right-click, Paste, and the Part Reference Prefix for the, for headers or for connectors is usually J. Press OK. When you are creating a symbol, you can use these icons, which are here, or you can use this Place menu, so click on Place, and I'm going to place some pins. So, left-click here, I'm going to name this pin as plus and this is going to be pin number 1, so I'm going to use number 1 here. Press OK, left-click, left-click, Escape. Select pin number 2, and change the name to minus. Left-click into empty space, click on Place, select rectangle, left-click, left-click, Escape, and make this outline little bit smaller, left-click to select it, press the left button, hold it down and move it. To zoom in, zoom out, use Ctrl, so press Ctrl on your keyboard and then mouse wheel. Zoom in, zoom out. I'm going to make it little bit nicer, I'm going to move this value maybe like this, and I'm going to move this J maybe like this. Select the value, just left-click here, and write 1x2 Header. Left-click into empty space, go to DigiKey, copy the part number, left-click, go back to OrCAD, and we are going to add this part number into Part Properties. So, left-click here, I'm going to call this new property like .ManufacturerPN. Left-click here, dot ManufacturerPN, and here we are going to place the part number. Left-click, Ctrl + V, and left-click here. This manufacturer part number property will be very useful, when we will be creating BOM, bill of material for our project. You will see later, okay? Left-click into empty space to unselect everything, and don't forget to save the library. When you have a look inside of our library, you will find there the symbol what we have just created. Okay? So, this is our header inside of our schematic symbol library. Next, we are going to create resistor, which we need for our schematic, so go to DigiKey, I'm going to use right-click, Open in new tab, we would like to search for resistor 360r 0805, Enter. Chip resistors, we would like to use this one, 1%, in stock, with 3D model, Apply, and this is the resistor what we can use. Copy this resistor description, left-click here, go to OrCAD, right-click on the library, select New Part, name is going to be the resistor description, right-click, Paste, and the prefix for resistors is R. OK. In our library, we are going to have new symbol, resistor symbol, and we are going to draw this symbol. Go to Place, select Pin, change the name to 1, number 1, press OK, left-click, left-click, Escape. Zoom in, press Ctrl and mouse wheel, switch off snapping to grid, just left-click on this button, Place, Line, and watch the position of my cursor, we would like to place the line somewhere in the middle between these snapping points, so the last number will be always 5, okay? So, left-click and watch now. Left-click. Do not move your mouse, left-click again, watch the numbers here, okay? Last number should be 5. Left-click, left-click, left-click, left-click, left-click, left-click, left-click, left-click, left-click, Escape. Left-click into empty space to unselect everything, and don't forget to switch on the snapping to grid again. Just left-click here. We are going to hide the pin name, just uncheck this, and also pin number, uncheck this. I'm going to make this outline little bit smaller, left-click to select it and move it, move the pin back, and move also this, and make it nicer. Move this and also this. Select value and put here 360R 1%. Go to DigiKey, copy the part number, left-click here, go back to OrCAD and in Part Properties, click here, left-click, add dot ManufacturerPN, Ctrl + V, left-click here. The last component what we need for our schematic is an LED. Go to DigiKey, right-click, Open in new tab, search for led 0603, Enter. LED Indication, we would like to use this one, in stock, with 3D model, Apply, we would like to use green one, Apply, and perfect. This is the LED what we can use. Copy the description, left-click here, go back to our project, right-click on the library, select New Part, right-click, Paste, I'm going to delete some of these text, because it's too long. Maybe like this. Change the prefix to D, OK. We are going to place pins, just left-click here, name C as cathode, number 1, press OK, left-click, left-click, Escape. Select pin number 2, change this to A as anode, left-click, zoom out, select this, make it little bit bigger, move the pins, left-click into empty space, switch off the snapping to grid, zoom in, draw or place line, and again watch the position of my cursor, so I'm going to draw it maybe from here, left-click, left-click, Escape. Now, use this icon Place polyline, left-click, left-click, press Shift hold it down, left, left, left-click, Escape. Here in Fill Style select Solid, left-click into empty space, we are going to draw the arrows, so again use this polyline, left-click, zoom in, maybe somewhere here, left-click, press Shift, hold it down, left-click, left-click, left, Escape. Left-click into empty space, place line, left-click, press Shift, and left-click, Escape. Select these, Solid, select whole arrow, just draw this selection rectangle, zoom out, move it maybe like here, Ctrl + C, Ctrl + V, and place it like here. Disable the pin name, uncheck this, disable pin number, uncheck this, left-click into canvas, enable the snapping to grid again, we are going to place line, left-click here, left-click, left-click, left-click, left-click, Escape. Make this smaller, move also this, and make it nicer. Move this value, and also this. Go to DigiKey, copy the part number, left-click, and you know what we are going to do. We are going to create new properties, left-click here, it's going to be called dot ManufacturerPN, and paste here the LED part number. Left-click, I'm going to change also this value, select it, and I'm going to put here Red. I know this LED is green, but little bit later, I would like to show you, how you can make some changes in your library, in case for example you need to adjust these symbols or if you made a mistake or something. Okay? So, little bit later we will correct this. Now, be sure everything is saved, okay? There, if it's not saved there is this star, so you can save this symbol, and also be sure the whole library is saved, so just select it and save it. We are ready to start drawing schematic, so double click on our schematic page, click on Place, Part, here select our library, and to place a symbol from our library into schematic, just double click on the symbol, okay? So, first the connector, double click and place it, Escape, double click on the resistor, press R to rotate, and left-click to place it, Escape, double click on the LED, press R on your keyboard to rotate, and left-click to place it, Escape. Maybe you notice these errors down here, for now just ignore them, okay? We have not created any footprints yet, later I will show you how to fix these. We are going to connect everything, go to Place, wire, zoom in, press Ctrl and mouse wheel, left-click, left-click, left, left, left-click, left-click, left-click, left-click, left, left-click, left, Escape. Place wire again, left-click, left-click, Escape, Place, we would like to place the power symbol, select this. We would like to use VCC_BAR, OK, left-click, Escape, double click, we would like to call it +3V3, OK, Place, ground symbol, we would like to use this one, OK, and left-click, Escape. When you hover cursor over a net, you will see its name. For example this one is +3V3. This one is GND. When you hover cursor over this net, it's going to have a weird name. And to name your nets, you can go to Place, and use Net Alias. Left-click, I'm going to call it DIODE1, OK, press R to rotate, and I'm going to place it on this net. Left-click, Escape. Now when I hover cursor over this net, it's going to be called DIODE1. Perfect. We have our schematic, and next we are going to create footprints. Footprints are used in PCB, and to create footprints, first we need to create pads. Go to Start menu, find Cadence PCB Utilities, and to create pads, we need to use this Padstack Editor software. Left-click. First, we are going to create pad or pin for our through hole connector. Click on File, select New, click here and be sure you are going to save this new pad or new pin into our project directory. I'm going to call it thru_pin, Save, here select Thru Pin, OK. I'm going to change units to millimeters, be sure circle is selected and Thru Pin is selected. Click on Drill, and here we need to put the hole size. Go to DigiKey, find datasheet of our header, open it and recommended hole size is 1.2 millimeter, so that's what I'm going to put here, 1.2, okay? There is no secondary drill, Drill Symbol I'm going to change this to circle, 1.2 millimeter, we can leave Drill Offset default, and we need to set these Design Layers. Basically here we are going to specify the size and shape of the pad, and in datasheet, there are no recommendations for the pad size, but this is what I normally use, so if you like, you can use exactly same dimensions. So, left-click here, instead of circle I'm going to use oblong, and the size what I'm going to use is 2 millimeter by 1.6 millimeter. This is how the pad is going to look. And we would like to have same pad on all the layers, so right-click, Copy, right-click, Paste, right-click, Paste. Go to Mask Layers, here we are going to specify the opening in solder mask layer, so solder mask layer is usually the green color on your PCB, and you don't want to have the green color on the pad, so here we are going to specify the opening. Left-click here, the opening is going to have same shape, it's going to be oblong as our pad, but it's going to be a little bit bigger, so here I'm going to put 2.2 millimeter and 1.8 millimeter. We would like to have this opening also on the bottom layer in the solder mask bottom, so right-click, Copy, right-click, Paste, click on Options, we are going to leave this default, click on Summary, and this is very important, don't use this Save which is here, you need to go to File and use this Save, okay? Left-click here. Very important. We are going to create pad for our resistor, click on File, New, I'm going to call it res_pin, here I'm going to select SMD Pin, OK. Be sure we are using millimeters, we are going to create SMD Pin and the shape is going to be rectangle. There is no drilling, click on Design Layers, and here we would like to put dimensions for our pad. Go to DigiKey, find the resistor, open datasheet, and we would like to see if there is some information about the recommended footprint. And it says here recommended footprint “Please refer to data sheet Chip resistors mounting”, I'm going to search for this. Here it is. And maybe here is some information, here it is. Okay? For 0805 resistor, the pad size is going to be C, D. Okay? So, it is going to be 0.9 by 1.2 millimeter. Let's go back, left-click here, rectangle, width is going to be 0.9, and the height is going to be 1.2 millimeter. Okay? So, this is the recommended pad size, go to Mask Layers, again we would like to make the opening around the pad, so left-click here, rectangle, make it little bit bigger than the pad size, so 1.1 by 1.4 millimeter, and also we would like to create this paste mask layer. This is basically the layer where solder paste is going to be placed. Okay? And usually this paste mask layer is exactly same as the pad. So, left-click here, use rectangle and the width is going to be same as the pad size, so 0.9, and height is going to be 1.2 millimeter. Options, we can leave this default, Summary, and don't forget to save. File, Save. We also need to create the pad for our LED, and you know exactly how to do it, click on File, New, I'm going to call it led_pin, select SMD Pin, OK, millimeters, rectangle, SMD Pin, there is no drill, click on Design Layers, go to datasheet, open it, the pad size is 0.7 by 0.7, so left-click here, rectangle, width is going to be 0.7 by 0.7, Mask Layers, left-click, make it a little bit bigger, 0.9 by 0.9, and we also need paste mask top, left-click here, and little bit later I would like to show you something, so instead of using exactly same size as pad is, I'm going to make it little bit smaller. Later we will correct it okay? So, I'm going to use let's say 0.6 by 0.6, oops 6. Click on Options, we can leave this default, Summary, and File, Save. There is one more thing what we would like to specify in this Padstack editor, and it is the via, which we will use in our PCB. So, click on File, New, I'm going to call it our_via, here select Via, OK, be sure we are using millimeters, Vias, circle, now left-click on this Drill tab, and the hole inside of our via is going to be 0.3 millimeter. There is no secondary drilling, drill symbol is going to be circle, 0.3 millimeter, Drill Offset leave this default, Design Layers, left-click here, and we are going to use circle and size of the via is going to be 0.6 millimeter. We would like to use same pad on all the layers, so don't forget right-click, Copy, right-click, Paste, right-click, Paste. When we click on the Mask Layers, we don't have to do anything here. We would like to mask the vias and there is no solder on the via, so leave this default, leave Options default, click on Summary, don't forget to save. File, Save. In the next step, we are going to create the footprints. So, click on this Start button, find the Cadence PCB and start PCB Editor. Select the license which you have, I'm going to use this first one and press OK. This is super important. Before you start doing anything in this Allegro software, we would like to add the local path into user preferences. Otherwise this software may have problems to find for example the pads, the pins what we have just created. So, go to Setup, User Preferences, and in Paths, select Library, in padpath left-click here, add new directory, just put here a dot, move it up, so it is on the top of the list, dot is local directory, okay? Press OK, OK, and switch off and switch on the software again. When the software starts, go to File, New, we would like to use Package symbol wizard, select it, click on Browse, be sure we are going to create the footprint in our project directory, I'm going to call it hdr1x2, Open, everything is correct, click on OK, we are going to start from this, this is very close to what we need, click on Next, here just load template, left-click here, click on Next, we would like to use mils, and the prefix for header is J, click on Next, number of pins is 2, pitch is going to be, I'm going to open datasheet, pitch is 100 mils, the width is 230 mils, and the length for 2-pin header is 200 mils. So, go back and this is going to be 100 mils, width is going to be 230, and the length is going to be 200 mils. Next, left-click here, we are going to find the pad or pin which we created for this footprint. So, just write thru, leave there the star and press Tab on your keyboard. You should see it here, left-click, OK, click on Next, origin will be pin 1 location, I'm going to select this, left-click, click on Next, origin means 0, 0 position in the footprint. Click on Next, Finish. This is the footprint which was automatically generated by the Wizard, and we are going to make some small adjustments. And as we work on the footprint and in the PCB I will explain what you see here and, and I will help you to understand little bit more how to work in Allegro, because there are many ways, okay, how you can work in Allegro. The simplest way is to use General edit. Left-click down here and select General edit. You need to use General edit, if you use something else, it may be hard for you to follow this tutorial, because you may see different menus in the options, okay? So, use General edit, right-click into empty space, Quick Utilities, Grids, I'm going to change this Non-Etch grid to 5 by 5 mils, OK. Now, I would like to place this rectangle, so use this command, left-click, go to Options, here you will see what you can do with this. We would like to place it on Package Geometry and silkscreen top layer, we would like to use or we don't want to fill this rectangle, and we are going to place it somewhere here. I'm going to open datasheet, and basically we are going to mark position of this, and this is pin number 1, so it needs to be on the left side, okay? So, zoom in, and I'm going to left-click here, and watch the position of my cursor, I'm going to maybe place it like here. Left-click. Right-click, Done. Now, we would like to move this designator. If you hover cursor over an object, then you will see some information. For example, you can see this is text, and it is on silkscreen top layer. So, we would like to move it, just use the Move command, left-click here, left-click on this text, and move it for example somewhere here. Okay? Left-click into empty space to unselect it. Now, we would like to move this designator, which is on assembly top layer, and this time when we will be moving this, we would like to hold the text in the center. So, select this, left-click, and place it maybe like here. Left-click. Left-click into empty space to unselect it, right-click, Done. We would like to mark pin 1 position, so I'm going to add text pin number 1 on silkscreen top layer, use this Add Text command, left-click, we would like to place it on Package Geometry silkscreen top, we would like to use size 4, left-click here, and just write 1. Right-click, Done. We would like to move it, so use the Move command, left-click, and move it maybe like here. Right-click, Done. Very quickly I'm going to explain how you can work with layers in Allegro. Click on Visibility, here you can switch off and switch on all the layers or you can enable and disable the most important layers. If you would like to work with all the layers, go on this or click on this button, left-click, and for example select Stack-Up, here you can see this is the top layer, so these are the pads on the top layer of our PCB, we can enable solder mask, you can see it is a little bit bigger than the pad, when we go to Geometry, Package geometry, we can enable silkscreen top, so this is usually the white color around the components, you can go inside of the Components, Reference Designator, and you can also enable the reference designator on the top. Okay? So, here you can enable and disable all the kind of layers which you need. For PCB manufacturing, we will need the mask layer, we will need the top and bottom layer, we will need the silkscreen and also paste layer. You will see when we will be generating the manufacturing information. I'm going to enable all the layers again, and we are going to continue. There is one more layer, which I have not mentioned yet, and we are going to use it. It is called assembly drawing layer, and on this layer, we are going to show the position of the components on our PCB, and also pin 1 location. In this footprint, for example this text is on assembly drawing layer. You can see assembly top. And here we would like to place a circle to mark this pin 1 location. So, use this Circle command, left-click, we would like to place this circle on Package Geometry, assembly top layer and left-click, left-click, right-click, Done. I'm going to show you how you can work with commands. So, you probably noticed if you would like to do something in Allegro, you always may want to use a command. So, if we would like to move this circle, we can make this Move command active and then we can select this circle and move it. Now, you can very simply recognize if a command is active, because when you use right-click, you will see this Done, Oops and Cancel commands here in this menu, and also other commands related to the command which is active. So, if you use Cancel, basically what will happen, all the changes what you did during the command, they will be canceled. I will make this move active again, I will move it, and I will move it again, now when I use right-click and do Oops, right-click, Oops, it will just go back like undo, but the command is still active, okay? And when you finish with your command for example when I place it into position which I like, left-click, you can use right-click and select Done. Okay? Now, no command is active, when you use right-click, you see the menu looks like this. In the next step, we are going to add 3D model into our footprint. Go to DigiKey, find our header, scroll down and here you can download 3D models. I know this is a Molex part and they usually have 3D models on their website, so instead of downloading 3D models from UltraLibrarian or SnapEDA, I'm going to find this on the Molex website. And I'm going to download 3D model directly from here. So, 3D Viewer and CAD Download, we would like to download step, let's say this one, and start and it's downloaded. This is the zip file what we have just downloaded, I go inside, and I'm going to copy this step file, I'm going to copy it into our project directory. Here it is. Go back to Allegro, click on this 3D view button, click on this 3D Mapper tab and in Model File, we would like to select the 3D model, so left-click here, select the file what we have downloaded, open. Wow! We need to correct the position, so use this button here, select it, left-click, and select the surface which is going to be placed on the top of the PCB. For example this. Left-click. You can use this MAN button, manually move the header around, we would like to rotate it, so we can use this left-click, and we would like to have the back of the header exactly here, because you can see here on the silkscreen this is the place where the back should be. Press Shift, hold it down, press middle button on your mouse, hold it down, you can move this 3D view like this. Zoom in, use mouse wheel or press middle button, hold it down and you can pan the view. To place these pins inside of this pads, you can use this XY button. So, left-click here, now left-click on the top of the first pin, left-click on the top of the second pin, left-click on the first hole, so where the first pin should go, and left-click on the second hole. Unselect this XY button and perfect. Press Shift, hold it down, middle button, hold it down, you can double check the footprint. You can go to Visibility, if you like you can uncheck everything, and you can for example only show the silkscreen top and you can have a look if the silkscreen goes nicely around the header. Perfect! Our footprint is finished, don't forget to save it, click on File and use Save or you can just click on this button here. We are going to create the LED footprint, click on File, New, I'm going to call it led0603G as green, select Package symbol wizard, click on OK, we would like to use this SMD DISCRETE as the starting point, it is very similar to what we need, click on Next, Load Template, left-click, click on Next, we would like to use millimeters, because datasheet is in millimeters, and the prefix for LED is D as diode. Click on Next, Terminal pin spacing, go to datasheet, and it is 0.7 plus 0.7, 1.4 millimeter. This E and D is 1.6, 0.8, so go here, put here 1.6, 0.8, click on Next. Pin, we would like to use the pin which we created for the LED, left-click here, leave the star there and just put here led, Tab, select it, OK. Click on Next, origin I'm going to leave center, because for SMD components, you would like to have origin in the place where the pick and place machine is going to pick up this SMD components, and usually it is in the center, so I'm going to leave it as it is, click on Next and Finish. We are going to add 3D model to this footprint, go to DigiKey, find our LED, scroll down, and here is the step file for the LED. This is the 3D model. Left-click, it looks like we can’t really download this file directly, so what I'm going to do, I'm going to select everything, Ctrl + A, Ctrl + C, go into our project directory, I'm going to create a new file, I'm going to call it led3d.stp, OK, and I'm going to paste the information about 3D model here. Save the file, here it is, and we are going to use it in our footprint. Go back to our footprint, left-click on this 3D view button, go to 3D Mapper, select Model File, left-click here, and select the file what we have downloaded, Open, and now we would like to place this 3D model correctly on our footprint. Basically, this is pad number 1, and this is the pad number 2. If we go back here, you can see this is the place around the footprint, okay? In the 3D model, it is this place, which is here. So, this is pin number 1, this is pin number 2. Go to datasheet, and this is pointing to the pin which is cathode. If we go into our schematic symbol library, then pin number 1 is cathode. So, basically this 3D model is rotated correctly, this is pointing to pin number 1, we just need to place it on the top of the PCB and move it on the pins. Do you remember how to do it? Click on this TOP, select the surface which is going to be on the top of the PCB, we can use manual to move this little bit away, I'm going to zoom out, press Shift, hold it down, press middle mouse button, hold it down, unselect MAN, select XY, left-click on this pin number 1, pin number 2, pad number 1, pad number 2, unselect XY. Okay? Go to Visibility, maybe uncheck this, and let's have a look if it's pointing correctly, okay? This is pin number 1, so this is cathode, and this is pointing correctly. We can close the 3D view. I'm going to hide these pin numbers again, and let's go back to our footprint. I'm not going to make any other changes in this footprint, because little bit later I would like to show you, how you can make changes in footprint, which is already used in PCB. Okay? So, this is definitely not the right footprint for LED, we will improve it later. However, what I would like to point out is this silkscreen and assembly drawing layer, this rectangle which is around the component. And when you think about this, this was created automatically by the component wizard, but ideally, we don't want to have silkscreen going through the pads. We would like to have the silkscreen and the assembly drawing layer around the pads. So, in the next step when we will be creating the resistor footprint, we will make this outline and assembly drawing little bit bigger. I will then tell you when we specify these dimensions. Okay, so this is everything for now for this LED footprint, you can save it and we can create the last footprint what we need. To create the resistor footprint, click on File, select New, I'm going to call it r0805, select Package symbol wizard, OK, we would like to use SMD DISCRETE, Next, Load Template, Next, we would like to use millimeters, and the prefix is going to be R, Next, Terminal pin spacing, go to datasheet, so this is the recommended footprint and the spacing between the pins, middle of the pins is C plus B, it is 1.2 plus 0.9, 2.1 millimeter. Put here 2.1 and this, we don't want to use the size of the component, as I mentioned before, we would like to maybe use something which goes around the pads. So, instead of size of the resistor, I'm going to put here numbers like 3.8 and 2 millimeters. Okay? So, the assembly drawing and silkscreen layer will not go through the pads, but will go nicely around the pads when we use these dimensions. Click on Next, select the pins for resistor, we call it res Tab, Res_Pin, OK, Next, we would like to keep the origin in the center, click on Next, and Finish. This footprint is almost perfect, maybe what we would like to do, we would like to move this text, so first I'm going to change grid, be sure you are in General Edit here, then right-click into empty space, Quick Utilities, Grids, I'm going to change Non-Etch grid to 0.1 by 0.1 millimeter, click on OK, and we would like to move this text which is on assembly top layer, we would like to move it inside of this component, so we are going to use Move command, we would like to hold the text in Body Center, hover cursor over the text, left-click and place it into center maybe like this. Left-click. Click into empty space, now we would like to move this text which is on the silkscreen top layer, we would like to hold it in origin, left-click on the text, and place it maybe like here. Left-click, right-click, Done. We can have a look on the individual layers of this footprint, just to check if everything is okay, left-click on this Color button, I'm going to switch off everything, select Stack-Up, now let's have a look on the top layer, so these are the pads, I'm going to disable them, let's have a look on the paste mask top layer, it is exactly same as the top layer, see? And the solder mask top is going to be little bit bigger like this. Also, what we would like to see is Geometry and Package geometry, silkscreen top, perfect, it is going to be exactly same as the assembly top, perfect, I can enable both, and we can go to Components, Reference Designators, and we should be able to see reference designator on assembly top and also on the silkscreen top. Everything seems to be fine. Only what is missing is the 3D model, go to DigiKey, find the resistor, scroll down, and we can download 3D model from SnapEDA website, left-click here, you need to register here to be able to download the 3D model, but it's free, so you can just register, go to 3D Model, and Download 3D Model. Here is the downloaded file, and I'm going to copy it inside of our project directory. Here it is. Go back to our footprint, go to 3D view, select 3D Mapper, Model File, left-click, this is the file what we have downloaded, Open, we would like to place it on the top, I'm going to move it little bit, it looks like it is placed correctly, but just in case, I'm going to use this XY, left-click, left-click, left-click, left-click, unselect XY, go to Visibility, I'm going to disable all these layers, and I'm going to double check if if the pads are nicely under the component. Looks good, perfect, we can close this. Our footprint is finished, don't forget to save it. We have created all the footprints, and now we need to assign these footprints to our symbols. If you go into our schematic, and when you double click for example on this resistor symbol, you will see that right now this PCB Footprint property is empty. So, we need to go inside of our library, and for each symbol, we need to specify the footprint, which is used with this symbol. Let's do it. Inside of our schematic symbol library, double click on the header symbol, go into our project directory, and I'm going to copy the name of the footprint. Go back into our library and paste the name into this PCB Footprint property. Double click on the LED symbol, go back into our project directory, I'm going to copy the name of the footprint, and I'm going to paste it here, and double click on the resistor symbol, go back to the project directory, copy it and paste it here. Don't forget to select the library and save it. Yes to all. The components which are used in our schematic, they are not used directly from our library. They are used from this Design Cache. So, what we are going to do, we are going to select connector, LED and resistor, just press Ctrl, hold it down and left-click on these symbols, and we are going to update this cache from the library. So, right-click on this selected symbols, and use Update Cache. Yes, yes. Once the cache is updated, we still need to update also the symbols, which are used in the schematic. So, when these three symbols are selected in the cache, right-click again, and now use this Replace Cache. Select this, Preserve reference designators and press OK. Go to our schematic, just double click, and I'm going to check if the symbols were updated, so double click on the resistor symbol, find the PCB Footprint property and here you can see, now there is the proper footprint name. Perfect. When these symbols were updated, you can see they don't look very nice, so what I'm going to do, I'm going to select it and press R to rotate, R to rotate, and now it looks nicer. Select the diode, R, R, R, R, it looks nicer, and let's try also this one, okay. Perfect. I promised to show you what to do, when you realize that there is a mistake in the schematic symbol, for example it says here this is a red LED, but it is actually a green LED. So, there is a mistake and we need to fix it. And we are going to do it exactly same way as what we use when we updated information about the PCB footprint. Inside of our schematic symbol library, double click on the LED symbol, we would like to change this value, so select it, I'm going to change it to green, now when this symbol is updated, select the schematic symbol library and save it. In the Design Cache, right-click on the LED symbol, select Update Cache, Yes, Yes, right-click on the LED symbol, select Replace Cache, select this, check this, OK, Yes, go into our schematic, and you can see the LED symbol was updated. I'm going to select it, press R to rotate, R, R, R, now it looks nice. Okay? So, this is the way how you can update the schematic symbols in case you find out there is something wrong and you need to adjust it. What can be very useful to know is how to annotate your schematic, and annotation is basically working with these reference designators. Okay? So, first you may want to know how to reset reference designators. Right-click on this project, select Annotate, select this, press OK, and watch what is going to happen when I press OK here. Remember now this is R1, D1, J1, and when I press OK, I reset the reference designators. R?, D?, J?. Now, we would like to annotate this schematic again, and we can do it automatically, just right-click here, select Annotate, select this, OK, and again watch what is going to happen when I press OK. We are back, this is now R1, D1, J1. This can be super useful, if you have like very big schematic and you would like to be for example sure each component has unique reference designator, so there are no for example two R1 resistors. We have finished our schematic, and we would like to be sure there are no errors, there are no warnings. And as I explained before, we are going to learn, how to fix this missing footprint error or missing footprint warning. You will get this warning when you try to place a symbol into your schematic. When I double click here, and when I place it into schematic, Escape, see? Now, there are four warnings. And to fix this, what we need to do, we need to add path into our project directory to the settings of this software. So, I’m going to use this Undo, and we are going to do it. I’m going to copy the path into our project directory, Ctrl+C, now, find where this Capture.ini file is located. Usually, you can find the location when you start OrCAD, then here in Session Log, this is where the Capture.ini file is located, okay? So, on my computer it is here, I’m going to open it, find this Allegro Footprints, and here we are going to add more directories. So, write Dir, I’m going to increase the number, so previous one is 1, I’m going to use 2 equals dot, this is just local directory, and I’m going to also add the project directory, so Dir3 equals, this is the project directory. Close this and Save. We have to do something similar also in this Allegro software, go to Setup, User Preferences, find Paths, Library, in padpath left-click here, we would like to add the path to our project directory, left-click here, left-click, this is where our project is located, just Choose, OK, and also for psmpath, left-click here, add, dot, and I’m going to move it up, and also add the project directory, left-click, and simply just Choose. OK. OK. And we need to close the software. So, I’m going to close this one, and also, I’m going to close this one. Start the OrCAD software again, open our project, and there should be no missing footprint warning anymore. Inside of our schematic page you can see the online DRC is empty, and when we try to place a symbol, see? No warning or no errors anymore. Perfect. To be sure there are no other warnings or other errors, we can run DRC check. Select this project, go to PCB, use Design Rules Check and Run. You can see there are no errors no warnings in this DRC, online DRC is empty and in Session Log, there is no mention of errors or warnings. So, this is perfect. Okay, we are ready to start working on our PCB. And I really hope I set up everything correctly, because this is the moment of the truth. We will see if everything is going to work. To start a new PCB, simply click on PCB and select New Layout. OK. I’m going to select this first license, you can use the license which you have and OK. I’m going to check if the component from our schematic were imported into this design, so click on this General Edit, and select Placement Edit. And yes, we can see the components from our schematic here. This is perfect, before we place them on our board, we are going to change some settings. Go to Setup, Design Parameters, click on Design, we are going to use millimeters, size is going to be A3, and this I’m going to change to -100, and also here -100. So, basically what we are doing, we are setting up the size of the canvas, so this is not size of our PCB, it is size of this black area, where we can work on our PCB, and this means that the origin is not going to be directly here in this bottom left corner, but it’s going to be moved little bit up. OK. We are going to draw shape of our board, I’m going to use General Edit, I’m going to place rectangle on Board Geometry, Design Outline layer, shape fill Unfilled, I’m going to start from 0, 0, left-click here, and the size of the board is going to be 20 by 20 millimeters. And very simple way how you can jump cursor into specific location, you can just go down here and write x, that’s the special command, and now write the coordinates. 20, space, 20, Enter. Okay? So, now we have this square with the size of 20 by 20 millimeters. Right-click, Done. We are going to change the grid, right-click into empty space, Quick Utilities, select Grids, for non-etch layer I’m going to use 0.5, Tab, 0.5 millimeter, OK. We are going to place components on our board, and the simplest way how to do it is click on Place, select Manually, select all the components, and just place them. Left-click, left-click, left-click, right-click, Done. To move components, we are going to use the Move command, and go into this Find tab, here switch off everything and only select symbols. So, we only would like to work with components. Left-click, move it maybe like here, left-click, if you would like to rotate component, right-click, Rotate, and just do it this way. If this doesn’t work, I’m going to do, left-click, if this doesn’t work go to Options, and here are some settings for rotation. So, sometimes this may be set for example to Absolute, you need to change it to Incremental, and here you can set the angle, so if I set let’s say 45 and when I use Rotate, it will be rotating with increment of 45 degrees. Okay? So, I’m going to change this to 90, and I’m going to place it like this. Left-click, left-click, right-click, Rotate, left-click, maybe I will do it like this, this, and I will move this little bit closer. Left-click, right-click, Done. Always when you are doing placement, watch these blue lines, they are telling you what pins need to be connected together. So, for example when you are rotating this component, you may want to rotate it the way it’s going to be easy to draw the PCB layout, it’s going to be easy to connect the pins together. To draw the tracks on this PCB, I’m going to use little bit more precise grid. So, right-click into empty space, Quick Utilities, Grids, and for all etch layers, for all the layers with copper, I’m going to set the grid to 0.1 by 0.1 millimeter. OK. Also, what we would like to do, we would like to set some basic rules, and we can do it in constraint manager, left-click on this constraint manager button, go to Physical, select All Layers, and here we are going to set the minimum track width what we would like to use in our PCB, let’s say 0.3 millimeter. So, select this, left-click here, and press Ctrl on your keyboard, left-click also here, and left-click also here, and we would like to set all these values to 0.3. Just write 0.3, Enter. Okay. What we would like to do, we would like to also select the via, which we created in Padstack Editor, that’s the via which we would like to use in our PCB, so left-click here, select this default via, remove it, in this filter write “our”, okay, this is our via which we created, double click, and press OK. Go to Spacing, select All Layers, and here we are going to select the distance between different objects on our PCB. If you double click here, you can see there are all the kind of ways how to specify all the kind of different distances between different objects, we would like to simply use 0.3 for everything, so I’m going to select all these values, just left-click to this first one, press Shift, hold it down, left-click on this last one, and I’m going to change it to 0.3, Enter. And do exactly same for this Same Net Spacing, select All Layers, left-click into this first one, press Shift, hold it down, left-click on this last value and just write 0.3, Enter. This constraint manager is very powerful, you can set here all the kind of different rules, so maybe little bit later, you would like to have a look, what you can do here. For now, this is everything what we need, I’m just going to close it, and we can continue. We would like to also check the stack up, so left-click here on this Xsection button, and currently we are using 2-layer PCB, and maybe what we would like to adjust is the thickness of the dielectricum, for standard 2-layer PCB this is 1.6 millimeter. Enter. Okay. Finally, we can draw some tracks on our PCB, and it’s super simple. Just use this Add Connect button, left-click, left-click on a pin, and just draw the track. Left-click, left-click, left-click, right-click, Done. If you would like to adjust this existing track, you can use this Slide button, left-click, left-click here, and just make it nicer. Let’s say like this, and right-click, Done. If in your Allegro something is working differently as what you can see in this video, then don’t forget to check three things. If you select a Command, then every command has different options. So, when I’m doing something, have a look if in your options there are no different settings. Also, double check this Find tab. If you can, if you would like to move for example a component, then you need to have the components or symbols enabled in this Find panel, so here basically, you are saying we, you are selecting the components what you would like to work with, and they have to be checked, otherwise, you can’t work with these objects. And the third thing, which is super important to check is this Edit mode. So, for example if you are using different edit mode as what I’m using in the video, your Allegro is going to behave differently. Let’s say I’m going to select this Etch Edit mode, and notice, that right now I don’t have to select any commands. I can directly draw the tracks. I can simply just left-click on a pad and draw a track. I can cancel this, I can simply just hover cursor over a track and move it. I don’t have to select these commands, because I’m in Etch Edit mode. And very similar, if you use for example Placement mode, you can guess, you don’t need to use any commands, you can just hover cursor over a component, left-click and you can just move it. Okay? By the way, if you would like to delete something, you can just use this button which is here, okay? So, use this Delete command, select what you would like to delete, right-click, Done. I’m going back into this General Edit mode, and we can continue. But don’t forget, if something is not working, check the Options, check the Find, and check the Edit mode, which you are using. Next, very quickly I would like to give you an example, how to work with this Find tab, and also how to work with the objects, which are already in your PCB. So, let’s say we would like to change the width of this track. Go to Find, switch off everything, now you can work with cline segments only, I’m going to check it, and then you would need to go and select every single segment of this track, press Ctrl, hold it down and left-click, or what you can do, you can use these Clines instead of these Cline segments, and then when you hover cursor over this track, all the, whole track is selected, you can just use left-click, and then, because we are in General Edit mode, we can use right-click, and you will see all the kind of commands, what you can do with this selected object. So, for example here you can see we can change the width of the track, left-click and let’s say we would like to have it 0.5 and press OK. Left-click into empty space to unselect everything. Okay? So, this is very simple way to explain, how to use this Find, and also how to use right-click to do some commands with the objects, which you already have in your PCB. So, let’s continue. I'm going to use Etch Edit mode, we would like to work with everything, and we would like to draw the track here which is 0.5 millimeter wide, we would like to connect it here, left-click, left-click, right-click, and we would like to add a via. Right-click, Done. I'm going to change the Etch grid, right-click into empty space, Quick Utilities, Grids, I would like to use 0.5 by 0.5 millimeter, OK, and now we would like to connect this via to ground plane, which we will place on the bottom layer of our PCB. So, we are going to draw a big ground plane on the bottom. Use this rectangle command, we would like to place it on the bottom, be sure the fill is dynamic copper and here select that we would like to connect this plane to ground net. OK. Now, simply just left-click somewhere here, and left-click. Right-click, Done. Very often when you are designing boards, you may find out that you need to make some changes in existing schematic, and then you need to transfer these changes to existing PCB, and that's what we are going to learn now. Go to our schematic, I'm going to copy this Ctrl+C, Ctrl+V, I'm going to place it maybe here, zoom in, I'm going to use Place, Wire command, and I'm going to connect it, left-click, left-click, left-click, left-click, right-click, End Wire, double-click on this net name, and we would like to call it DIODE2. OK, and these are the changes what we would like to import into our PCB. Select our project, save it, go to PCB, select Update Layout, here you will see a list of the changes what is going to happen, and click on Sync. Go to Allegro, click on Place, select Manually, select all the new components, and we would like to place the diode on the bottom side of our PCB, so right-click, select Mirror, and right-click, Rotate, left-click, left-click, right-click, Mirror. Mirror will place the component on the bottom side of the PCB, and right-click, Rotate, we need to rotate it like this. Left-click, left-click, right-click, Done. I'm going to adjust the shape of the ground plane, use this Shape Select command, left-click, left-click on the ground plane, hover cursor over the edge of the ground plane, press left button, hold it down, move it, right-click, Done. When in Etch Edit mode, go to Find, be sure everything is on, so left-click here, zoom in, use mouse wheel, left-click, we would like to make this track wider, go to Options, select line with 0.5, left-click, left-click, left, left, left, left, left-click, left, I'm going to move this, just hover cursor, press left button, hold it down and move it. Left-click, left-click, perfect. Now, do you remember when we were creating this LED footprint, I told you this is not a proper footprint, and now is the time to fix this footprint. Okay? So, let's say during PCB layout, you found out that one of your footprint is wrong, and you need to make some changes in this footprint. And that’s what we are going to learn now. Go to File, Recent Designs, find the footprint for our LED, here it is, left-click, yes we would like to save our PCB, and let's fix this. First, we are going to fix this paste layer in the LED pad. Basically, when we were creating this pad, we intentionally made this paste layers smaller, so we can learn how to update pad in a footprint in case there is something wrong. Here you can see this is the mask layer, which is little bit bigger than the pad, this is the pad, and this is the solder layer, which should be exactly same size as the pad is, and it is not. So, we need to fix it. Go to Padstack Editor, click on File, select recent pads and open LED pin, left-click, go to Design Layers, and check what is the size of the pad, 0.7 by 0.7 millimeter. Go to Mask Layers, left-click on the paste mask, and we are going to correct the width, it is going to be 0.7 and 0.7 is also the height, so this is the right size for the opening in the paste mask layer for this pin. Don't forget to save it, so click on File, Save. Go back to our footprint, then click on Tools, select Padstack, and here you can use Replace in case you are going to completely use different pin or different pad, or in our case, we just can use this Refresh. So, watch what is going to happen, okay, the size of this paste layer should be same as the pad size, so basically it will disappear. I'm going to select this and Refresh. Refresh, Close. And it is fixed. I have just updated my Cadence software to the latest version, so it looks a little bit differently as what I had like 10 seconds ago, but it is still very similar, it is basically the same, so if you are using different version of this software don't worry, you still will be able to follow the tutorial. So, let's continue, I'm going to change grid, right-click into empty space, Quick Utilities, Grids, and I'm going to use 0.1 everywhere, so 0.1, Tab, 0.1, and also for All Etch 0.1, Tab, 0.1, OK. I'm going to delete these lines on top silkscreen layer and on top assembly drawing layer, so use the Delete command, go to Find, switch off everything, enable lines, hover cursor over this line on assembly top, left-click, left-click into empty space, hover cursor over the line on the silkscreen top, left-click to select it and left-click into empty space to delete it. Right-click, Done. We are going to draw the rectangles again, but a little bit bigger, so use this Shape Add Rectangle command, left-click, go to Options, we would like to draw on package geometry, silkscreen top layer, we would like to use unfilled rectangle, now left-click here, and maybe one, two, three, four, left-click. I would like to mark where cathode is located, so we are going to place one more rectangle, this time we'd like to use static solid, so it's going to be filled, and left-click, left-click, right-click, Done. I marked this side of the footprint, because this is where pin one is located, and when we have a look into our schematic symbol, and when we enable these pin numbers, you can see the cathode is where pin one is located. Okay? So, that's the reason why we made this marking where pin one is. We need exactly same shape also on the assembly top layer, so I'm going to use this Copy command, left-click here, go to Find, switch off everything, we would like to work with shapes, select them, in Options we would like to use this User Pick, so left-click here and left-click, right-click, Done. We would like to move this on assembly top layer, so select it, right-click, change to assembly top, left-click into empty space, and I'm going to use Move command, I'm going to select this, and we are going to move it up here. Left-click, right-click, Done. What we are going to do next, it is not really necessary, but let's make this footprint properly, so we are going to make these shapes which are on boundary layers, we are going to make them same size as this outline. So, let's do it. I'm going to use this Color button, left-click here, switch off all the layers, go to Geometry, Package geometry, enable DFA boundary top and silkscreen top, OK, go to Shape Edit, and just hover cursor over this corner, move it, hover cursor here, press left button, hold it down and move it. Go to Color button, Geometry, Package geometry, uncheck this and Place boundary top layer, enable this, click on OK, and do exactly same. Just move this and also move this. Go to Visibility, enable all the layers and go back to General edit mode. I'm going to make this text on assembly top layer little bit smaller, just hover cursor over the text, right-click, Change Text block to number 2, and left-click into empty space to unselect it, we would like to use Move command, in Options use Body Center, left-click, and move it maybe like this. Left-click. Right-click, Done, and we can move also this, so I'm going to use Move command again, I'm going to use Symbol Origin, and we can move this. Left-click, left-click, right-click, Done, I'm going to open 3D view, just double check if everything is okay, press Shift, hold it down, press middle button on your mouse, hold it down and okay. These pads are correctly placed on the footprint, this is the marking of the cathode, and on the 3D model this supposed to point to the part with cathode. Everything seems to be fine, I'm going to close this, and don't forget to save your footprint. Go back to our board, click on File, Recent Designs, this is our board, and we are going to update the footprint, so watch what is going to happen with this diode footprint. Click on Place, Update Symbols, we would like to update all footprints, you can update only the LED, but I'm going to update all of them, and I'm going to also reset symbol text location and size. Check this, Refresh, watch. Perfect! Close and the footprint of our LED was updated. We are going to make the silkscreen layer and assembly drawing layer a little bit nicer, basically we are going to move this reference designators little bit, so go to colors, we are going to switch off some layers, so we can see the text little bit nicer, disable top and bottom layer, and in Geometry, Package geometry we would like to maybe hide the boundary layers, this one, this one and also here, this one, this one, OK. Now, use the Move command, in Find, switch off everything, we would like to work with text, left-click on this text, right-click, Rotate, left-click, left-click, left-click, right-click, Rotate, and left-click, left, left, right, Rotate, left, left, left, right, Rotate, left, left, right-click, Done. And we would like to also rotate the reference designators on the assembly drawing layer, be sure you are in this General edit mode, be sure no command is active, and then in Find, switch off everything, we would like to work with text, and then when you hover cursor over a footprint, then you will see the text on the assembly drawing layer. And you can see, this one has the letter D on the bottom, and this one has the letter R on the top. And we would like to have it same way, so just use right-click and Spin, right now it is spinning the way which is not what I would like to have, so go to Options, and we would like to spin around Body Center, select this, okay now this is what I would like to have. So R is on the bottom, D is on the bottom, D is on the bottom, and here R is on the top, so we would like to rotate this, right-click, Spin, left-click. Left-click into empty space to unselect everything. We are going to add some text on the silkscreen top layer, so we use this Add Text button, left-click, here select Board Geometry and silkscreen top, we would like to use a text size 3, just use this arrow or you can write the number here, and left-click, write plus, left-click, write minus, and left-click, write FEDEVEL Academy. Or you can use your company name. Right-click, Done, we would like to use Move command, so left-click, we would like to work with text, left-click, I'm going to move it, maybe I would like to hold it in Body Center, so I'm going to move it here, and I'm going to move this here, and I would like to hold this in Symbol Origins and place it here. Left-click, right-click, Done. And your PCB is finished. Well done! If you would like to see 3D model of your board, you can just click on this button, then you can say wow! If you would like to change colors go to Setup, Preferences, let's select blue, OK. If you would like to play with the individual layers, you can do it here, or if you need to update 3D models of the components, or if you need to add some 3D models into your board, then you can do it here. Okay, perfect! Next, we are going to create views, which you can find very useful, when you will be doing PCB layout, but you can also use these views to generate documents for PCB manufacturing. And this is how you can create views. Click on this Color button, switch off all the layers, enable top layer, go to View, Color View Save, and we are going to call it top layer (TOPL). Save it, now go back to the colors, I'm going to disable this, enable bottom, call this bottom layer (BOTL), save it. Go back to colors, disable bottom, we would like to create a view for silkscreen top layer, so in Geometry select Board Geometry, enable silkscreen top, in Package Geometry enable silkscreen top, and also in Components, Reference Designator enable silkscreen top, I'm going to call this view silk top (SILT), save it, do exactly same for the bottom silkscreen, so disable this, enable, disable, enable, disable, enable, call it silk bottom (SILKB), and few more very simple layers, switch off everything, go back to Stack-Up, enable solder mask top, I'm going to call it solder top (SOLDERT), now disable, enable, I'm going to call this solder bottom (SOLDERB), do exactly same for the paste layers, paste top (PASTET), paste bottom (PASTEB), and I'm going to create one more view, disable everything, and in Geometry, Board Geometry, enable design outline, this is the board outline, so I'm going to call it BOARD. Save, we can close this, and if you like, you can also close this. I don't need to save it. If you go into Visibility, here in this View, you can select the views which we just created, so very quickly if you would like to see let's say silkscreen top layer, just select it. Okay? So, this is silkscreen top. If you would like to see the silkscreen bottom, this is silkscreen bottom. By the way, if you would like to see how your board looks from the bottom view, you can go to View and use this Flip Design, okay? So, now you can very nicely read all the text on the bottom side of your board. View, go back. If you need to see all the layers, simply just click on On. Before we start generating documents for PCB manufacturing, we would like to be sure, there are no errors on our PCB. And to check if there are any errors, you can simply just right-click here, and select this Display Status. Everything should be green. Okay? Sometimes, this may be red, you can just use this button Update All, sometimes this can be red, you can just manually Update DRC, left-click here, and perfect. Everything is green, there are no errors, press OK. When you are running design rule check, you need to be sure, that the rules what you are using, they are actually checked. If you go into this Constraint Manager, then Analyze, Analysis Mode, here you can see a list of all the rules and you can see if they are going to be checked or not. For example, if I click on this Spacing, you can see almost everything is on, so almost all these rules are going to be checked. But if I select Silkscreen, you can see everything is off, so right now when I run designs rule check, basically no silkscreen errors are going to be found, because they are not checked. Okay? So, when you will be using designs rule check, you need to go through this, and be sure you enable everything, all the rules which you are using in your design. In case there is an error, this is how it is going to look. First, I'm going to save this, and let's say we are going to route this track very close to this pad, and you can see there will be error, because the cursor shape is different. Left-click, right-click, Done, so this means there is an error. If you go down here, Display Status, you see there is shorting error, and you can also left-click here, and it will tell you where exactly it is located. You can also use these Tools, DRC Browser to find all the errors, which are on your board. You can simply double click here, and here it is. Okay? So, this is very simple way to find out what kind of errors you have on your board in case you need it. I'm going to load our project again, and let's continue. We are ready to generate the outputs for manufacturing, and the first files what we are going to generate are called Gerber files, and this is how you generate them. Go to Manufacturer, select Artwork, and here we are going to specify all the layers and all the combinations of layers, which we need to generate the files, which are needed to manufacture your PCB. For this we are going to use the views which we already created, so to create the output or Gerber file for top layer, we need to select this top layer view (TOPL), and this is what they need to manufacture the top layer of your PCB. Okay? We can simply add this into our list, just use right-click, select Add, and call it TOPL. OK. If you go inside, you will see here are all the layers, which are enabled here. And same way, we can add all the other layers. But first, I'm going to remove these default layers, just use right-click and Cut, right-click, Cut. I'm going to select the bottom view, right-click, Add, call it BOTL. The next one is going to be silkscreen top, right-click, Add, SILKT, then silkscreen bottom, right-click, Add, SILKB. Next one is going to be solder top, right-click, Add, SOLDERT, I'm going to copy this, OK. Solder bottom, right-click, Add, Ctrl + V, B, and paste top, right-click, Add, Ctrl + C, OK, paste bottom, almost done. OK, and also, we would like to add here the board outline layer, right-click, Add, BOARD. There are two more outputs, which we would like to add here, these are assembly drawing outputs, and we will not generate Gerber files from these outputs, but we will print them to PDF. Click on this Color button, inside Geometry, Package Geometry enable assembly top, in Components, Reference Designator enable assembly top, now right-click, Add, I'm going to call it assembly top (ASMT), OK, go back to colors and disable assembly top, enable assembly bottom, select Package Geometry, disable top, enable bottom, and right-click, Add, call it assembly bottom (ASMB), OK. If you like, go inside and double check if there are all the layers. I would like to save all this work, basically when you press Cancel, you will lose all these changes what we made here, so I'm going to use OK, this will save it, and I'm going to open it again. There are couple of settings which we would like to adjust here and the very important one is this Undefined line width, we would like to set it to 0.1 millimeter for all outputs. So, select the first output and I'm going to put here 0.1. I'm going to copy it, Ctrl + C, select the next one and put here 0.1. Basically, what we are doing, maybe you noticed in your board, there are number of lines with a 0 line width. They are very thin, and if we would like to print them, they would not be visible. Okay? So, here we are setting up that if there are some lines with a 0 width, then 0.1 millimeter will be used instead. And then we will see them in the outputs, okay? So, that's what we are doing now. And the last one, perfect. Next, I'm going to select this assembly drawing top layer, and I'm going to set this priority to one, and for the assembly drawing bottom layer I'm going to set this two. This can be useful when you are printing these assembly drawings into PDF, then you specify on what pages you would like to have them, so they are in correct order. First on the first page there would be top layer and on the second page the bottom layer. Also, for assembly drawing on bottom layer, we would like to have it mirrored, so don't forget to check this. Go to General Parameters and I'm going to leave everything as it is, I'm going to leave it default. We are ready for a very important moment, we are going to generate the Gerber files, go to Film Control, Select all, uncheck the assembly drawings, and Create Artwork. Scroll down, and you can see there are some warnings on silkscreen top layer, if you go up, then you will notice they are not really important. These are basically just messages about replacing the lines with 0 width, replacing them with 0.1-millimeter width. Perfect! Now, let's have a look on the Gerbers what we have just generated. To check the files, I'm going to use software which is called ViewMate, and this software is completely free, if you like you can download it and you can install it. Once you start the software, this is how it looks. Go to File, Import, Gerber, go to our project directory, I'm going to copy the path to our project, Ctrl + C, by the way these are the Gerber files what we ve generated, the files with art extension. Go back here, Ctrl + V, Enter, I'm going to order these files, I'm going to select the first one, left-click, and then the last one, press Shift, hold it down, left-click. Press Ctrl, hold it down, unselect this, Import, and these are the Gerber files. I'm going to switch off everything, I'm going to enable the board outline, double click here, and let's have a look on top layer, just double click. Double click to disable it, solder top, silkscreen top, paste top, you can also combine the layers like this. Okay? I'm going to disable this, and let's have a look on the bottom layer, paste bottom, silkscreen bottom and solder bottom. Perfect! The next file what we would like to generate is called NC Drill file, go back to our project, Manufacturer, NC, NC Drill, and this is important. Check this Auto tool select, go to Parameters, check also this and also I'm going to use these English units. OK. And left-click on Drill. To check this file, go back to our Gerber viewer, select the empty layer, then File, Import, Drill, and this is the file what we have just generated, select it, Import. I'm going to enable the board outline layer, use mouse wheel to zoom out, and as you can see, the drilling is in right position and also it has the right size. Perfect. If you would like to print for example assembly drawings, you can go back to our project and use File, Export to PDF, we would like to export assembly bottom and top, I'm going to leave everything else default, I'm going to leave this default, Page Setup I'm going to use millimeters and A4, scale let's say 5, width is going to be 2, and height 2, and I'm going to change this prefix, I'm going to put there LED Project. Click on Export, go to our project directory, open the PDF what we have just generated, and this is how it looks. Okay? On the first page, there is the assembly top layer, and on the second page, there is assembly bottom layer. In case you just need simply print something from Allegro, you can do it this way, go back, I'm going to close this, I'm going to enable top layer, and let's say we would like to print this, because we would like to manufacture this PCB at home, and we need this top layer. So, go to File, select Plot Setup, I'm going to use scaling 1, and I'm going to use black and white. OK. Click on File, Plot, basically plot is print, so left-click here, here you can select where you would like to print, I'm going to use PDF, OK, I'm going to call it top layer, Save, go to our project directory and open the PDF what we have just created. Okay, super simple. So, this is what you would use if you would like to manufacture this PCB at home. Go back to Allegro, and the next file what you will need to build this board is called pick and place. Go to File, Export, select Placement, simply click on this Export button, I'm going to close this, go to our project directory, and I'm going to open this file which we just generated. Inside of this file, you can see there is location of all the components, which are on our board, and you can see there is also rotation and the site if they are on top or bottom layer. Next, we would like to print our schematic, go to OrCAD, and in case you need to change some settings for printing, you can go to Options, Extended Preferences, Schematic and you can choose here the theme for printing, I'm going to use this light, and also what you may want to do, go to Options, Preferences, and you may want to uncheck the grid, because you don't want to see the grid in the printed schematic. It can be really disturbing. Then select the project, go to File, Print Setup, I'm going to print into PDF, so this is okay, go to File and select Print. Just press OK, I'm going to save it into our project directory, I'm going to call it Schematic, Save, go to our project, I'm going one directory up, because we are inside of the Allegro, here is the schematic, I'm going to open it, and here it is. The last file what we would like to generate is BOM, bill of materials, go back to our schematic, and in the BOM, we would like to use this .Manufacturer parameter, which we included in every symbol which we created. So, go back to our schematic, now select our project, go to Tools, use Bill of Materials, and here we are going to add the parameter, so I'm going to copy this, Ctrl + C, Ctrl + V, and I'm going to write here .ManufacturerPN. Okay? So, this will when we will be creating table with BOM, this will add the manufacturer PN into this table. Here I'm going to name the column for the manufacturer part number, I'm going to call it Manufacture PN. We would like to open it in Excel, so check this and press OK. Here it is. I'm going to make it a little bit wider, so you can see it better, so this is our BOM, bill of materials, you can see we are using three types of components, and here is the column with the manufacturer part number which we included in our symbols. Perfect. And our project is done. In case you would like to download the finished project, you can just go and search for Fedevel GitHub, click here, go to youtube-cadence-quick-tutorial or you can go directly to this URL, this is the whole project, you can simply download it, just left-click here and download. If you would like to learn more about electronics, we have number of online courses, just search for Fedevel Academy, click here, and I have created number of basic and also very advanced courses. You can find them all listed here, or you can go to our Marketplace, and you can find there also courses from different people, courses about KiCAD, EMC, measurements… I really hope you found this tutorial useful, I would like to thank you very much for watching, and see you next time. Bye!
