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    Solidworks Help - Boxed Control Arms
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    Senior Member JD66's Avatar
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    I'm planning to design a boxed lower control arm soon. Some of the plates will have bends in them, which means I will need the flat pattern in order to send off to laser. Has anyone dealt with this in Solidworks?

    I realize I can do the bent plates as separate part files and use the sheetmetal tools to flatten it (in order to get a 2D profile for laser cutting), but I prefer to design the entire arm as a single part where each extrusion is an individual plate to be cut. Anyone dealt with plate work that needs a flat pattern? I'm basically trying to make a flat pattern from one feature in the model tree of a part.
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    Re: Solidworks Help - Boxed Control Arms
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    Millenium Member plkracer's Avatar
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    Can you make multiple part bodies in a single part is SW? That's how I do it in catia. It treats each one as individual, but you can tie geometry back to any other part body. Then you can copy that body into a new one and flatten the sheet. Works great for weldments because you can boolean them at the end, and run them through analysis immediately (if you do that sorry sorry thing).
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    Re: Solidworks Help - Boxed Control Arms
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    I think Plkracer's idea is the best approach. Weldments can be a real pain to maintain flat patterns of details, yet still allow for adding features like fillets, etc. at the weldment level. An old trick we used to do is to create an assembly and have that represent the weldment leaving all the detail parts intact (created however you like). If you can create assembly features at the weldment assembly level, that could work as well. Depends on what your needs are....its been years since I used SolidWorks.....so my insight on that application is limited.
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    Re: Solidworks Help - Boxed Control Arms
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    You can do a multiple body sheet metal part. I have done an example of exactly of what you are trying to do. You've can have it if you want.
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    Re: Solidworks Help - Boxed Control Arms
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    The Wizard bdkw1's Avatar
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    Make an assembly first, then draw your parts in the assemble drawing. Then if you make a change in the assembly drawing, all the parts will update along with it. Unbending is pretty simple from there to make DXF files.
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    Re: Solidworks Help - Boxed Control Arms
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    Senior Member JD66's Avatar
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    Cool, thanks guys. I'll play with it this week and let you know what route works best
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    Re: Solidworks Help - Boxed Control Arms
    #7
    Millenium Member plkracer's Avatar
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    The company we usually work with on weldments likes bdk's way of structuring the parts, since we work in catia, and they work in SW, and Dassault can't seem to get the two to cooperate. If you transfer a step file over, it doesn't carry the individual part bodies, but keeping everything in one part is a ton cleaner when a weldment is 100 unique plates, if you keep the part in its native file.

    Working with master geometry in an assembly file works, you can link to external geometry in catia, and keep a link to it, but you need to load the entire assembly to update it properly.

    On a side note, I use the surfacing work bench to offset slots to allow some room for the tabs. Make it a lot easier to use boolean removes on a plate to make the slots, then offset the intersecting surfaces, from which you can make a flat pattern. It updates much nicer than the other method, and you only need to draw the tabs.
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    Re: Solidworks Help - Boxed Control Arms
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    Senior Member Jerm's Avatar
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    It does seem easier at first to just draw all your parts in one file using separate bodies for each piece, but if you use the assembly structure it works much better for kicking out drawings and sending to the fab shops. If you start with an assembly, then start drawing new parts in the assembly, just like separate bodies, it will end up working better in the end. Just remember that after one piece is drawn, start a new part. Each piece is a new part file.
    With this method you can also easily see how many common parts you can use, as you can insert that same part many times in the assembly and use in different locations.
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    Re: Solidworks Help - Boxed Control Arms
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    Senior Member JD66's Avatar
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    I've been designing control arms as part files since it's easy to adjust a single dimension (say the arm length grows by 1/2"), and all of the bodies update. With separate part files, I'd have to adjust dimensions on several parts in order for the assembly file to be correct. It probably takes longer to get the DXFs all sorted out from multiple body part files, but it's not too big of a deal.

    After messing around in SW, I found I can create a separate part from a body of the control arm part file. There will only be a few bodies in the control arm that need to be bent, so I'll create new parts from those bodies which I can then make a flat pattern of using the sheetmetal feature. Should work well enough for what I need.
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    Re: Solidworks Help - Boxed Control Arms
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    Senior Member SamR's Avatar
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    Quote Originally Posted by JD66 View Post
    I've been designing control arms as part files since it's easy to adjust a single dimension (say the arm length grows by 1/2"), and all of the bodies update. With separate part files, I'd have to adjust dimensions on several parts in order for the assembly file to be correct. It probably takes longer to get the DXFs all sorted out from multiple body part files, but it's not too big of a deal.
    If you make each feature a new part within the context of an assembly you can reference each part as if they were features in a single part. Eg: say you wanted to make a L bracket out of two flat pieces. Open a new assy, insert new part, edit part and make the first piece of the L. Insert a second new part, use one face of the first part as the sketch plane, do a convert entities on an edge that is on the plane (or make a line coincident and dimension) then draw the rest of the piece off of that. Now when you update the length of part one the length of part two also updates.

    The way you're doing it works fine though just makes a few more files to keep track of. I believe that's how most people are getting tube layouts out of SW as well.
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