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Is it possible in OnShape yet to pattern a hole cut into a part?

Phil_G_1987Phil_G_1987 Member Posts: 4
I've been creating a C-channel cross member, this cross member has holes cut into it at 100mm increments, the only way I could find to do this was to sketch each individual hole in a single sketch and then use the Extrude -> Remove tool to create the holes.

I was looking for a tool or a way of being able to just pattern the hole Extrude feature and not pattern the entire part multiple times.

I tried using the Boolean tool but I couldn't seem to get it to work.

Phil

Best Answer

Answers

  • Phil_G_1987Phil_G_1987 Member Posts: 4
    @BruceBartlett I'd never even thought to select the inner face. Thankyou!
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,459 PRO
    I have a hole not going through. I tried to pattern "Face of Extrude 2" with Face pattern checked, chose Front plane as axis (should go align Y), step 160mm, 3 steps --> Linear pattern 1 is red and hovering gives error: "Linear pattern 1 did not regenerate properly: Pattern could not be created on the same part."

    Any ideas?
    //rami
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 632
    Rami said:
    I have a hole not going through. I tried to pattern "Face of Extrude 2" with Face pattern checked, chose Front plane as axis (should go align Y), step 160mm, 3 steps --> Linear pattern 1 is red and hovering gives error: "Linear pattern 1 did not regenerate properly: Pattern could not be created on the same part."

    Any ideas?
    You need to select all of the face associated with the hole, including the cap face at the bottom of it if it isn't a thru-hole and any filleted faces.  I would suggest using a pocket selection if isn't a thru-hole to get the faces (RMB -> Create Selection) or box select.

    The other potential issue is that the direction of the pattern might be going in the opposite direction.  If your selection is correct, try toggling the flip direction and see if the pattern works.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,459 PRO
    Ok, got it - thanks.

    Now I have 8 holes in a row and I wan't to mirror copy them to the other side. Can't select from feature list to pattern/mirror - so I need to zoom and select each of them 2 clicks per hole (+10% missed clicks and fixes)

    Wouldn't it be more convenient to have feature pattern / mirroring instead or in addition to face pattern/mirror?

      
    //rami
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 632
    3dcad said:
    Ok, got it - thanks.

    Now I have 8 holes in a row and I wan't to mirror copy them to the other side. Can't select from feature list to pattern/mirror - so I need to zoom and select each of them 2 clicks per hole (+10% missed clicks and fixes)


    If the holes are truly patterned, then take advantage of the "Select patterns" option of our "Create selection" tool.  This will pickup all of the faces that are identical to the selection you've created rather than forcing you to select them N number of times.




    3dcad said:
    Wouldn't it be more convenient to have feature pattern / mirroring instead or in addition to face pattern/mirror?
    I think feature and face pattern and mirror is something that can and should coexist.  One isn't a one-to-one substitute of the other.  Feature pattern/mirror is something that we know needs to be in Onshape.
    1.png 185.9K
    2.png 200.9K
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • 3dcad3dcad Member, OS Professional, Mentor Posts: 2,459 PRO
    @jramlsey Having both face and feature pattern/mirror would be the best solution. And if it was possible to automatically choose without checkboxes (maybe have advanced tab for forcing one or another) which one to use - it would be nice and simple. Personally I like to use feature tree to make selections for feature pattern/mirror to know exactly what I have selected. 
    //rami
  • brucebartlettbrucebartlett Member, OS Professional, Mentor, User Group Leader Posts: 2,102 PRO
    edited March 2015
    Nice tip @jramlsey, Only thing that took me a while to workout is the "create select tool" is on the RMB most of the time. This will come in real handy.

    A quick key for this would be good eg. Shift Spacebar, don't know if that's possible.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • stg434stg434 Member Posts: 19 ✭✭
    I am having understanding the workflow for using, in this case, the circular pattern tool. I have been successful in patterning a hole through a part but not an open feature say a v-groove on the surface of a part.  Onshape says "Circular pattern 1 did not regenerate properly: Pattern could not be created on the same part."

    For the pattern setup I chose face pattern and picked both of the angled faces, I then chose the fillet edge.  No joy, I tried several different combinations but no joy.


  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 632
    Hi Stg434,

    I can't completely tell what you are trying to do based on the picture you attached but I am assuming you made v-groove through the entire top face of your part and tried to circular face pattern it.  If this is true, the faces you are circular patterning would intersect with one another causing the number of faces to be generated to change and fail.  A way to do it in this case would be to pattern parts that would result in the v-groove then subtract them with a boolean

    1. Create a part that would etch out the v-groove.  Start a circular pattern and select the part for "Entities to pattern"


    2. Select the circular edge to get the axis of rotation.  Configure the rest of the pattern to get the right number of instances and angle between parts/overall angle and accept it.


    3. Start a boolean, choose "Subtract" and put in all of the patterned parts for the tools.  Since these were just created by the circular pattern I either use cross-selection to get the parts from it or shift+click in the parts list to get a batch selection.


    4. Select the part that you want the v-grooves in it as the target




    If my assumption is wrong and you do have end cap faces, then face pattern is reasonable.  You need to make sure you select all faces that need to be patterned, including the end caps.

    1. Start a circular pattern and choose the "Face pattern" option.  For the "Faces to pattern" select all of the faces that need to be patterned.  In the image below, it is three faces: the two faces for the v-groove and the face that is used for the end-cap.


    2. Select the edge of the face you want the v-grooves to be in to get the axis of rotation.  Enter the number of instances and the angle between faces/overall angle you want to pattern.  Keep in mind, if the angles are too low then the faces will start to overlap and can't be created.


    I hope this helps
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • stg434stg434 Member Posts: 19 ✭✭
    Thank you for the feedback jramlsey - very thorough!  Unfortunately still no joy.  Initially I tried this on a SW part I uploaded and thought it might have something to do with the imported solid so I modeled in Onshape.  Attached is a better pic to show the problem.  There are only 2 faces to pick in contrast to your example.

    I didn't think about the parts version.  I'll have to try that but was wondering why the face pick failed.

    Cheers
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 632
    Hi Stg434,

    Sorry I can't be of more help, however I do see the issue (I think).  The faces you are trying to pattern aren't capped by a face.  As a result, the faces that are being patterned are extended beyond/to the center of rotation causing the faces to intersect.  It is something I will talk to the development team about on Monday.
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
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