How to model an easy part for CNC machining in FreeCAD - Product Design - Flowwie & sliptonic

hello everybody thanks for tuning in to this video i have 10 000 subscribers here on my freecad academy channel which is absolutely incredible so therefore it's super nice to see this great support i decided to give something back to you and for this video i teamed up with brad collette who you might know under his name sliptonic he is not only the author of free cat books and an expert in the field of manufacturing a field where i am definitely not an expert and we decided to make two videos brad made one video i make one video about the product design process from the first prototype to the complete manufactured part we will start in this video here showing you how to design the first prototype in every single detailed step go to the next step develop the second prototype where you see some of the geometry has dramatically changed how do you make these changes in freecad without destroying your whole part and for the next video in the series you have to switch over to brad's channel and watch the video on how to manufacture the part so i wish you a lot of fun with this video let's go i will now show you the modeling process in every detailed step which can be a great exercise for learning freecad and the freecad part design workbench so we start with a new file clicking on file new so please make sure that we are here in the part design workbench and we click on the combo view in the tasks tab create a new body and under the new body we create a new sketch by clicking on create sketch we select as a sketching plane the x y plane here go to ok and then we are in the sketcher workbench so let's start with the basic geometry of the grind plate we will start with a rectangle rectangle we click on the horizontal axis here and click here to make it complete right click the next thing we need to do is to delete this edge here so select it click on delete on the keyboard the next thing we need to do is to give some basic dimensions we click on the horizontal distance button the upper edge here and click 142mm then we click on the vertical distance on this edge here and we define 25 millimeters the next thing we want to do is we want to make this geometry symmetric to this green vertical axis therefore we select the upper corners here the vertical axis and click on symmetric now the last thing we need to do is to define where this point is located we just glue it on the horizontal axis by clicking the fixed point onto an object command so now we have a fully defined geometry and can continue our sketching next thing i want to make is to create a radius down here for the grind area so i click on end points arc select these two points here and define the arc now we need to define where this center point of the arc is located just glue it on the vertical axis center point vertical axis fixed point onto object and we're fine the next thing is to define the radius click on radius constrain a radius command click this radius and define 30 millimeters the position of the center point is not yet defined therefore we click on vertical distance between the sketch origin point and the midpoint of the radius and define 26 millimeters then we have to close the geometry select the line tool and just connect these two points and these two points and the first basic sketching is done so we click on close can click the pad command here pad the selected sketch look in the model tree that the sketch is selected click on the pad command six millimeters and as you see we will have the first basic shape of the grind blade finished there are two slot holes here in the grind plates that go through the whole geometry so we can define these two slot holes also in the original sketch so we open the pad here again go to the first sketch and define the slot holes therefore just simply create a slot in the sketch define the slot to be located here and the next slot here right so let's make the radius of both slot holes equal to each other select both radius here go to the radius command do you want to share the same radius yes i want 3.5 millimeters i need to enter comma here because it's the german edition of frequent so don't be fooled okay so um the next thing let's make sure that these slot holes are in the same height so vertically let's align them vertically we can easily create a line click on the construction geometry command you will see that the line now is blue and connect the two outer points of the slot holes with each other right click and as you see that happened automatically freecad set this line to be horizontal because it was only in a very slight angle and so frequent thought it would be a good idea to make this ma make this automatically if it did not happen to you like for instance like this let's see it would look like this then you could click this construction line and set it to horizontal constraint manually and then you need to define where the slot holes are positioned let's start with the vertical distance from this center point to the sketches origin point 12 millimeters let's define the width of a slot hole here 20 millimeters here the same 20 millimeters now let's define the length of this line here 116 millimeters and it's not yet symmetric you see there is one degree of freedom left so just click on this and this point here select the vertical axis and go to symmetric and now the sketch is complete let's click on close the sketch has changed we now have two slots in the sketch that go through the whole geometry next thing we need to do is to create two other slot holes that go 2.5 millimeters into the geometry to make room for the screw heads so let's define a new sketch x y plane okay go to the section view and now we don't want to refer on 3d geometry so in the model view we can hide the pad by clicking the space bar and make our original sketch visible also by selecting it and clicking the space bar now we see the first sketch but no longer the 3d geometry we are currently in sketch 001 and in this sketch we can simply click the command create an edge link to an external geometry and link these two arcs into the new sketch then we go to another slot slot and slot we know that this distance here has to be 20 millimeters same here let's set the radius equal to each other yes 7.5 millimeters radius let's check in the tasks tab that the sketch is fully constrained go to close enable the pad hide the original sketch and now you will see that the sketch is somewhere down here it's on the wrong side of the geometry so the sketch should be up here on the top and we can achieve this easily by selecting the sketch go to its properties select attachment position and make the z positioning here six millimeters so it will change from down here six millimeters up here and now is located on the upper side of the geometry and now we can select sketch zero zero one and make a pocket create a pocket two point eight millimeters deep okay and now we have this nice shape let's rename a few things here to make it less confusing sketch is now named basic shape and pocket i rename it as lark large slot okay so we're pretty much finished with the design so the next thing i want to make is to create a chamfer on this edge here i simply select this edge go to chamfer and as you will see the chamfer ends here so we need to add these edges also to the chamfer area go to add and click these two edges so we have three edges now size of two millimeters chamfer okay and now the geometry is chamfered the next thing i want to make is to create fillets on these corners here so select these two edges fill it four millimeters at the last thing i want to fill it these edges here fill it four millimeters and okay so that is my first prototype slip toning in this video will tell you that this operation first creating the chamfer and then fill it here will create a surface that cannot be easily done with machining and therefore we will have to change this geometry here in the next steps so after some testing on my skate with a 3d printed prototype and after some email conversation with sliptonic i decided to make some changes on my first prototype and i will show you all these changes in detail and that's a very important and very interesting part of the video because that's something that occurs very often when designing a product that you have to make changes on your 3d model this can cause some problems here and there in freecad and i will show you how to handle these problems so let's start with the first iteration the first thing i wanted to change is the overall height of the model if we click on the right side here you will see that the dimension in z direction here is six millimeters and we want to change that to five millimeters that's pretty simple we only need to change the first pad double click on it and change the six millimeters to five millimeters and then we change the height of the whole part problem is we still have the sketch for the pocket the large slot sketch here is located still at a c value of six millimeters and so we could change this manually but we can automate this very easily by clicking on large slots and change the position here from six millimeter a fixed value we click on the formula editor here and now we define it as the pad length pad length is the value of my first pad the length and whenever i change the length here this will be automatically inserted in the z valve here let's try it if we had eight millimeter thickness here you will see that the large slots placement is at eight millimeters so you can automate this very easily and therefore you don't need to manually change it next iteration is the basic shape i need to change the basic shape i'll click on it and make some changes i will change the 142 millimeters width to 150 millimeters i will change the height of the whole part to 26 millimeters that works pretty easily without any problems i change the appearance of the slots here only 14 millimeters wide i don't need them to be as large as they used to be um radius is okay the 12 millimeters here is okay yeah everything looks pretty fine right now for me but i need to change the distance 116 here will now be 124 millimeters to make the slots sit a little bit more on the outside here close it yep everything looks fine the only thing that i don't like is the appearance of the large slots here so i need to change these as well it's the 14 millimeters distance that has to change here you could automate this as well if you like to so okay that looks pretty good um let's delete the fillet because sliptonic said that there is problems with manufacturing of the fillet here so i kill it and i kill the upper fillet as well and the chamfer next thing i want to do is to change the shape of the groove down here therefore i have to edit the basic shape this is the only change that i have to do that could cause some problems let's see what happens when i do these changes when i go to basic shape sketch i will now delete completely the whole radius down here this could cause some errors let's find it out what happens nothing so far that's pretty good um i have now these two points down here i will add a 18 millimeter radius here and make the transition from this edge and this edge into this radius less sharp and filleted so this could be a little bit tricky let's find out what happens we start with another radius with the end points here we put it somewhere around here set it to 18 millimeters and now let's create some fillets that go from the edges into my new radius first thing i set the center point of this new middle radius on the vertical axis here and then i start another arc going from here to there something like that and another arc next thing is the tangent constraint that i need to set between this edge and this radius also between these two radius here and here and there and then we will have a look at our degrees of freedom what we have to eliminate so we have three degrees of freedom so far that pretty good we define the distance between these two points in horizontal distance 50 millimeters so we have two degrees of freedom left yeah we could click these two ready and say equal and as a last step i set this center point below the center point of my sketch six millimeters so that's the next shape appearance we will see what happens now i go to close and you see that the slot holes here the larger slot holes do something incredibly stupid and that's because freecad still in version 19 has some problems with the so-called topo naming problem topological naming and as you remember i defined the large slots to be defined about these arches here and as you see this went terribly wrong after the major changes that i did in the underlying sketch so when i select this sketch you see that now no longer this and this radius is taken from the other sketch by the linked edge command here but it's now this radius and this radius here and therefore the sketch looks terribly off so i first thing i need to delete these two and have to define it myself again so i would recommend not using this command linked edge to avoid these problems in the future to make the whole construction more stable so let's work with the construction geometry link these two set them to 12 millimeters in vertical now we need to define the horizontal position and the length of the construction geometry here therefore we close the sketch go in the basics shape sketch and we will see this here i click it and i name it x xdist you see xdist is the new name of this dimension here then i close the base sketch go to the large slot sketch again and i use the variable from the other sketch therefore i select the construction line here go to horizontal distance and go to the formula editor then i need to insert the label of my first sketch that's um basic shape under basic shape we enter constraints dot x disk that's the name that i just defined in the other sketch 124 millimeters okay okay and now i need to make those two symmetric to the vertical axis here close now i repaired the large slots here and made it more stable towards further changes whenever i change this basic shape here i no longer work with the linked geometry of these two radius here but i work with a more independent sketch now as the last step let's add the fillets then you press v and three on your keyboard then you get this wire frame drawing style here you can select these four corners easily select fillet four millimeters v1 to make the drawing style as before and then we could add a little chamfer on top of this here chamfer one millimeters and we are good so that's the second prototype and it should be a little bit more stable than what we created as the first prototype after watching this tutorial you might ask yourself what's the purpose of the just designed part and i will show you this in a second here that's me doing one of my absolute favorite sports rollerblading grinding on a steel rail and especially for grinding on rough surfaces like concrete or something like that i use a grind plate on my skate frame to protect the frame from extreme abrasion on the frames plastic check out slip tonic's video on how to manufacture the part you should check out sliptonics patreon page where you can become a member and support him and his work with a monthly donation so if you like to see a professional cam environment infrequet it would be very good to support slip tonic if you don't have patreon you can support him under liberapay liberapay sliptonic you find him here under his real name brad collette and you can donate here so thank you very much for watching have a good time and see you next time goodbye

Channel: Free CAD Academy

Views: 29,024

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Id: zVl9B3rtZtc

Length: 24min 24sec (1464 seconds)

Published: Sun Jul 18 2021