Creo Parametric - Sheetmetal Bends (Part 1)

in creo parametric sheetmetal the bend command is one of the most powerful and commonly used commands and there's a lot to this command both in the ribbon and the various different tabs so in this video we're going to cover the commands in the ribbon the placement tab the BEM line tab and we'll briefly touch on been lounge and the properties tab will save transitions and relief for another video and there's so much in here that I actually want to jump over to a couple of slides real quick to explain some of the different options that you have in here first let's take a look at some of the different options that you have in the ribbon and this first group of icons allows you to choose the bend side whether the Bend side is going to be on one side of the Bend line the other side of the bed line or it's going to be about both sides of the Bend line then we have a flip icon that allows us to change which side is the fix side then we have a couple of buttons over here that allow you to toggle the type whether you're doing an angle Bend or a roll Bend and with an angle Bend you're going to specify both the angle and the radius of the Bend with the roll Bend you're just going to specify the radius of the Bend and it's going to bend to the remainder of the material on the Bend side so when you choose that you're going to do a roll Bend you're gonna notice that the bend angle control and how you're measuring the bend angle both of these areas are going to be grayed out and so just as I mentioned this is the bend angle that you would specify for an angle Bend and then this drop down list allows you to choose how you're going to measure the bend angle whether you're going to measure the internal angle which is the other control from here or the one that's currently shown is the deflection from straight and these are complimentary angles to one another so for example if you have a ninety degree Bend that's the same whether you're measuring the internal angle or deflection from straight but if your deflection from straight was 45 degrees then your bennett angle would be a hundred thirty five degrees the next area in the dashboard allows you to specify the bend thickness and there are default values of thickness and thickness times two and of course you can enter in the value and the last control that we have here on the dashboard is how you're going to measure the bend angle whether you're measuring the bend angle to the inside of the bend which I generally find more common because that's how sheet metal bending machines work but alternatively from the drop-down list you could choose whether you're going to measure the bend angle to the outside of the bend and a third choice is to use sheet metal parameters which I'll touch on at the end of this video the next important aspect to talk about is how you're going to place the sheet metal and if you go to the placement tab there's a collector that allows you to specify either the bend surface or a bend line and the Bend line would be a pre-existing sketch or curve that you would want to use and you could choose that Bend line from the placement tab if you choose an actual Bend line then the Ben line tab is going to be grayed out in addition if you choose that Bend line there is a box that you can check in order to offset some distance from that Bend line that you have selected alternatively from the placement tab instead of selecting the Bend line that you want to use you could select the surface that you want to use and if you select the surface that you want to use then the Bend line tab will be available and from the Bend line tab you could choose either to sketch your band line or you could choose to use drag handles in order to locate your but the ends of your Bend line both ends of it on a reference and then dimension it from additional reference and so you have controls for two ends of those men lines with that explanation let's now jump into creo parametric and see how to do this all right I am in creo parametric I'm starting off with a very simple part in order to walk you through these different choices to create a sheetmetal Bend here you can see the command for it right on the ribbon in the model tab I will click on it you'll notice that the placement tab is in red and in this situation first we'll take a look at selecting the surface that we want to bend and the different options that are available so let's say I want to bend this surface over here it selected everything else in the placement tab is grayed out right now and be aware when you're selecting a Bend surface you only have one surface that you are able to select and you can see that we have these different controls over here that allow us to define the bend line but we before we do that I'm going to sketch the Bend line I can define an internal sketch and here it throws me into sketch mode I can hold down the right mouse button an add in an additional sketch reference and pick that surface over there let's close out of that dialog box then I can sketch in a line and for this first one for some of the different things I'll show on the ribbon I'm just gonna make a horizontal line for my Bend line and let's change this dimension let's use a value of nine I'm happy with my sketch I can hold down the right mouse button and from the pop-up menu here I can choose the check mark in order to complete out of sketch mode so now you can see a preview of the geometry that's being created and you'll notice that it shows this side over here as the fixed side and it's bending over here I can click on this arrow and if I hold my mouse over the arrow usual pop a blue hint to tell me what this is confer controlling but I'm not seeing it so if I click on that you'll notice that that allowed me to flip which side is the fixed side so in this case here if this is fixed it's bending the bigger amount of material but if I flip it then it's keeping this side fixed and it's flipping this section over here and it's the same as clicking this button on the dashboard now could the preview can be a little bit confusing sometimes but it is toggling back and forth which one is being fixed and I want the big section to be fixed so I'm gonna flip it once more let's take a look at some of the other different controls and before I do the other different controls I'm going to increase the radius in order to make some of these other different controls a little more obvious to you I'm going to use a big thickness and right now it has it's indicating that we're using the sheet metal parameter for the thickness I'll show you where those different parameters are but I'm going to enter in a big value a value of 1 and so we can see where the bend line is and right now the bend is entirely on one side of the Bend line if I can click this button you'll notice that it will Bend up to the Bend line let's click this other button this one puts it symmetric about the bend line so here we can see our Bend line and it's symmetric about it and just to flip it again here's one side and here it's being right on the bend line so those are those controls right now we are set to use an angle Bend so we're defining the bend angle here you can see that we have a value of 90 degrees if you go to this drop-down list you can change the angle for example here is 30 degrees let's go to 60 degrees or you could enter in a value for example if I wanted this to be 70 degrees from this drop-down list we're choosing whether we are measuring the resulting internal angle or if we want to measure the deflection from straight a slight correction to a mistake I made during the initial recording of this video here we have our angle of 90 degrees from this drop-down list we can see that right now we are measuring the resulting internal band angle if I change to this button over here you'll notice the angle changes to the other side and now instead we are measuring the bend angle deflection from straight let's say I change this from 90 degrees to 45 degrees let's type in the value so we're measuring the angle from deflection from straight if we now change to measuring the internal Bend angle you can see that the been flipped so it's maintaining 45 degrees but it's 45 degrees from the surface measuring the internal Bend angle if I wanted to be out over here instead I would change this to 135 degrees the complement of the initial 45-degree angle from here we have the radius that we specified and this drop down list allows you to specify whether you want to measure that radius to the outside surface of the bend or if you want your sheet metal parameter that's called SMT D FLT default radius side to control whether you're inside or outside but again we will use the default for the inside and let's change this back to it at an angle of 90 degrees and that way we have our Bend being created in the model so that is a very simple example let's hit the check mark there you can see our bend that is located in here I am going to take this and suppress this because I'm gonna go and create another sheetmetal Bend right now let's create our sheetmetal Bend and again I'm going to select the surface that I'm going to Bend if I go to the placement tab again you see if this is selected and everything is grayed out I'll go to the Bend line tab and instead of sketching we're going to use references and for the references you can just grab these different draggers and drag them out so I'll drag it to this edge so it's going to be located on that edge now I have this other drag handle to control what I am dimensioning from let's drag it up to over here and there we can see that we have a dimensional value and I can change this to a value of two for the second side we can grab this and drag it to what we want the reference for the location of the end of that bend line let's grab the other dragger and I can drag and say I want to measure from that edge over there and has right now value let's change this to a value about eight so I'm going to end up having an angle Bend line and you can see that right now it's choosing this side as the fixed side I can flip it and so this side is now fixed and this is the side that's going to be bent and you can see I can drag it up over here through the different the range of motion to see the preview that I would end up getting let's change this to 45 and there you can see it bent at that particular angle so that is the alternative way of locating the bend line where you're grabbing those different references let me hit the check mark and I'm going to jump over to my other model in order to show you and the alternative method of defining the bend line in this model I have a flange wall and then I mirrored that wall so I actually have two distinct walls over here but I created a sketch that is across both of those surfaces and these two surfaces are coplanar so you want to bend multiple surfaces one requirement that you have is that they are coplanar let's choose to create a bend and right now I had the sketch selected let me cancel out of here let me deselect everything if I click the bend command now I can go to the placement tab and instead of selecting a surface to Bend I will select this sketch and you can see that it is been again it's using the wrong side that I want for the fixed side I want to flip the fixed side and so now it's keeping the main piece of the geometry straight and here I have the ability to control the angle that I want to bend it at let's again make this a much bigger value for the radius that I am using right now we're using a value of 0.5 let's make it bigger let's use a value of 1 because I want to show you a roll Bend and I have my radius of 1 if I click this button over here it's gonna bend to the end of the material let's go and keep on dragging over here and so by using the roll Bend it's just gonna roll out to the end I don't have the angle control to specify how much I bend it it's just starting the bend in rolling to the end of the material so that is good oh yeah one other thing to show you since I selected the bend line let's check the box over here to offset the bend line so now I have this additional dragger and you can see that as I dragged it too low the preview one away indicating that it was curling up on itself too much and it was going to end up in the self intersection but if I drag it up over here you can see how much material is left in order to Bend and let's just offset this let's try a value of 0.125 yeah that looks good and a couple of other tabs that I'll mention here there is a transitions tab I'll cover that in a different video here we have a relief tab as well I'll cover that in another video but we have our bend allowance and our bend allowance allows you to calculate the developed length as I mentioned in other sheetmetal videos if you're not a sheet metal manufacturer really no point in entering a value in here or managing it let your sheet metal manufacturers figure out what is the developed length for the blank that's going to be used in order to create your part they are the profession they've got the heuristic data they've got the information they'll be able to calculate that really if you're not a professional not worth your time from the properties tab this is another location where you can change the name of the material so I am going to hit the check mark for some of the different options in the sheet middle I mentioned that there there are parameters available to different ways in which to find those first off if you go to your model properties dialog box which you can get to from file prepare model properties but it's command that I use so often that I have it in my click access toolbar let's click on model properties here we have a sheet metal group since this is a sheet metal part here is the Benz line I'll click the blue change hyperlink for Benz and in the sheet metal preferences dialog box you can actually jump to the other sheet metal preferences in here and you have three different controls here we have the bend radius and from the drop-down list you could choose some value here we have thickness two times the thickness half the thickness that's the default Bend radius but of course you can change it and here we have the bend radius side inside or outside if you wanted that measure to the outside surface you could use this radio button instead and here we have the default Bend angle and some predefined values but you could enter in what value that you wanted for the default Bend angle and as I hover over these different things you can see that it tells you the name of the corresponding parameter in other words this one is SMT sheet metal DFL default Bend angle and here this is the sheet metal default radius side and here's the sheet metal default Bend radius let's click OK to get out of here next we can go to our parameters dialog box and you can access the parameters from the same model properties dialog box or if you click the close button to get out of model properties you can also access parameters from the model intent overflow menu on the model tab you can also go to the tools tab and right on the ribbon you have a parameters command and since this is a sheet metal part it has a number of parameters automatically in here and those same three parameters that we saw in the sheet metal Preferences dialog box we have here in the parameters here we have our sheet metal default Bend radius and right now is locked because it's using a relation that has that equal to the thickness here we have the sheet metal default radius I'd set to inside and here we have our default Bend angle which is set to 90 and here we can see that this is the result of a relation we cancel out of here then go to our relations dialog box again because this is a sheet metal part we have a number of different relations that automatically come in here and see the information and so here we have that which one was that I was looking at here the sheet metal default Bend radius is equal to the sheet metal thickness if you don't want this in here you could comment out this line using a forward slash and an asterisk then we can click the ok button out of there if I go back to my parameters then we should see that the sheet metal default Bend radius is a numerical value it's no longer locked by a relation the source still is sheet metal though I hope you enjoyed this video for more information please visit w-w-w it a thumbs up and if you like this video please click the subscribe button to be informed when new videos are uploaded thank you very much

Channel: Creo Parametric

Views: 38,515

Keywords: creo parametric, ptc creo, creo ptc, creo parametric tutorial, creo parametric 2.0, creo parametric 2.0 tutorial, creo parametric 3.0, creo parametric 3.0 tutorial, creo parametric 4.0, creo parametric 4.0 tutorial, creo parametric 5.0, creo parametric 5.0 tutorial, creo parametric 6.0, creo parametric 6.0 tutorial, creo parametric sheet metal, creo parametric bends, bends in sheet metal, sheet metal in creo

Id: auHnVeODh9E

Length: 19min 24sec (1164 seconds)

Published: Wed Sep 11 2019