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nsgoldberg10-Marble
10-Marble
March 30, 2020
Solved

Extrude from two perpendicular sketches

  • March 30, 2020
  • 3 replies
  • 6743 views

Does Creo have a way to use two perpendicular sketches to create a part? The attached image shows the two sketches, and the final image shows what I'm looking for. I created the final part by making an extrusion, then by making an extruded cut.

 

I have some complex geometry on a part where it would be easier to have creo simply use the two sketches to find the intersecting geometry and create a part in one step. I swear I've done this before, but can't seem to figure out how to do it now.

 

Thanks in advance.

Best answer by LndoVnBtchmrk

I created a subroutine UDF that works.  You load the UDF, select one sketch, select the other sketch, and you're done.  It creates two extrudes: one creates solid geometry, the other cuts it.  I've never created or used these before so I don't have much advice.  Take a look at this post.

 

This post is showing as a reply to LukaszMazur, but it was a reply to nsgoldberg's reply to me.  But when I edit the post it says it's in reply to nsgoldberg?  Khoros bug?

3 replies

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LndoVnBtchmrk12-Amethyst
12-Amethyst
March 30, 2020

You can use the Intersect feature with those sketches to create a composite curve.  But I don't think you can use that to fill the inside volume.

Have you tried a user-defined feature?

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    nsgoldberg10-MarbleAuthor
    10-Marble
    March 30, 2020

    No, I'm not familiar with a user-defined feature. I'll have to check that out.

     

    I tried intersect but couldn't find a way to make it a closed volume.

    L
    LndoVnBtchmrk12-AmethystAnswer
    12-Amethyst
    March 31, 2020

    I created a subroutine UDF that works.  You load the UDF, select one sketch, select the other sketch, and you're done.  It creates two extrudes: one creates solid geometry, the other cuts it.  I've never created or used these before so I don't have much advice.  Take a look at this post.

     

    This post is showing as a reply to LukaszMazur, but it was a reply to nsgoldberg's reply to me.  But when I edit the post it says it's in reply to nsgoldberg?  Khoros bug?

      P
      Pettersson15-Moonstone
      15-Moonstone
      March 31, 2020

      I'm having trouble understanding the problem. Why is doing this in one feature better than doing it in two? What are you trying to gain by it? The example obviously doesn't need this functionality.

      You can generally get this effect by extruding the sketches as surfaces and then merging them. In Creo 7 we'll get multi body capabilities, so you'll be able to do it by extruding each of them and then combining them with an intersect. today you can do this if you make them as separate parts and merge them together.

      I never found any real need to use things like this, however. What's the problem with just doing it with two extrudes?

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        LukaszMazur16-Pearl
        16-Pearl
        March 31, 2020
        Just a quick ideas, as I haven't had time to test them.
        1. I would try to create a datum graph feature using the upper portion of the longer sketch (projecting edges to graph) and then a sweep of the rounded sketch with trajpar control.
        2. One extrude of the rounded sketch in both sides and then an extruded cut based on the longer sketch.

        As far as I know you won't be able to use two sketches simultaneously to create one extruded feature, you will need to combine at least two features.
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