Welcome to the Onshape forum! Ask questions and join in the discussions about everything Onshape.

First time visiting? Here are some places to start:
  1. Looking for a certain topic? Check out the categories filter or use Search (upper right).
  2. Need support? Ask a question to our Community Support category.
  3. Please submit support tickets for bugs but you can request improvements in the Product Feedback category.
  4. Be respectful, on topic and if you see a problem, Flag it.

If you would like to contact our Community Manager personally, feel free to send a private message or an email.

Holes not lining up?

Hi. I am an occasional user of Onshape for small diy projects. I am working on a simple drawing with 4 parts mated together. There are 2 holes in each of 2 parts with a bush between them at each hole. One set lines up perfectly but the other doesn't. All the parameters are the same so I can't understand what is wrong. Any ideas?
https://cad.onshape.com/documents/5b3df14cccf95f03ae8ab887/w/6e4f40fcc04778bb37a2dd45/e/eb6106a87e31d3de3e0c36e5?renderMode=0&uiState=64165d9c3fb17b4c3df3e61f

Best Answers

  • steve_shubinsteve_shubin Member Posts: 1,061 ✭✭✭✭
    edited March 2023 Answer ✓
    @riccardo_ingrosso

    https://cad.onshape.com/documents/a1ef3f00a65c62a51f3596ef/w/f046564d95fdfa5187d1d4de/e/b7310393e275d33d7672865c

    I saw your part studio prior to your fix. Something on the left was not 50 mm from the left edge. It was 49.xx

    Take a look at the part studio in the document in this post

    I sketch one point and then mirror across the right plane. Then use one HOLE feature to make all the holes



  • nick_papageorge073nick_papageorge073 Member, csevp Posts: 619 PRO
    edited March 2023 Answer ✓
    https://cad.onshape.com/documents/c13a608ef1a02cab542c1e51/v/10c1cfd97a1b63880e249c41/e/1d9329456667bf6c2d6d194a?renderMode=0&uiState=64171a993c265c40a7f69fdb

    Try modeling it this way. The way you did it is not taking advantage of what OS can offer. The differences:

    1) The parts are modeled in the positions they will be assembled at. This allows you to design in the clearances/contact the way you want between parts. It also allows you to share sketches for multiple parts (like the hole sketch).
    2) It allows you to use one feature to make the hole through all the parts.
    3) The parts are modeled symmetrically about the default plane. This allows the mirror to work for the second set of holes. Generally a good idea to model symmetrically.
    4) No chance for things not lining up, like you ran into with a dimensioning error.

    In the assembly:
    1) All the parts come in at their intended locations. That means you just need to "fix" one, and group the rest.
    2) Only one mate needed for the second roller.
  • riccardo_ingrossoriccardo_ingrosso Member Posts: 8
    Answer ✓
    That’s a great reply Nick and very informative to me. I certainly would never have worked out that bit about the mc’s being based on the centre of mass. 
    The tip about placing everything in the sketch is also very handy. Thank you. 

Answers

  • riccardo_ingrossoriccardo_ingrosso Member Posts: 8
    So I found a workaround and got my holes lined up but I'm still unsure why it didn't work the first time around. I based everything from a central mate connector and used offsets to position holes and parts but for some reason they ended up slightly out of line. I would still like to understand why, if anyone can shed some light on this for me.
  • steve_shubinsteve_shubin Member Posts: 1,061 ✭✭✭✭
    edited March 2023 Answer ✓
    @riccardo_ingrosso

    https://cad.onshape.com/documents/a1ef3f00a65c62a51f3596ef/w/f046564d95fdfa5187d1d4de/e/b7310393e275d33d7672865c

    I saw your part studio prior to your fix. Something on the left was not 50 mm from the left edge. It was 49.xx

    Take a look at the part studio in the document in this post

    I sketch one point and then mirror across the right plane. Then use one HOLE feature to make all the holes



  • riccardo_ingrossoriccardo_ingrosso Member Posts: 8
    That makes sense! I don't know why I didn't think to use the mirror feature. Thanks for the response.
  • nick_papageorge073nick_papageorge073 Member, csevp Posts: 619 PRO
    edited March 2023 Answer ✓
    https://cad.onshape.com/documents/c13a608ef1a02cab542c1e51/v/10c1cfd97a1b63880e249c41/e/1d9329456667bf6c2d6d194a?renderMode=0&uiState=64171a993c265c40a7f69fdb

    Try modeling it this way. The way you did it is not taking advantage of what OS can offer. The differences:

    1) The parts are modeled in the positions they will be assembled at. This allows you to design in the clearances/contact the way you want between parts. It also allows you to share sketches for multiple parts (like the hole sketch).
    2) It allows you to use one feature to make the hole through all the parts.
    3) The parts are modeled symmetrically about the default plane. This allows the mirror to work for the second set of holes. Generally a good idea to model symmetrically.
    4) No chance for things not lining up, like you ran into with a dimensioning error.

    In the assembly:
    1) All the parts come in at their intended locations. That means you just need to "fix" one, and group the rest.
    2) Only one mate needed for the second roller.
  • nick_papageorge073nick_papageorge073 Member, csevp Posts: 619 PRO
    As to your original problem of the holes not lining up, the reason is the way you dimensioned them. You selected an implicit mc within the hole feature. The mc finds the "center of mass" of a surface. So when there were zero holes on the surface, it found the exact center of the part, and you offset 200mm from it. But after you made the first hole, and while you were making the second hole, the "center of mass" of the surface is no longer the center of the part. The first hole removed material, and the center of mass shifted. That is what led to the holes not lining up. See screenshot the two explicit mc's don't line up. Try it you'll see.


  • riccardo_ingrossoriccardo_ingrosso Member Posts: 8
    Answer ✓
    That’s a great reply Nick and very informative to me. I certainly would never have worked out that bit about the mc’s being based on the centre of mass. 
    The tip about placing everything in the sketch is also very handy. Thank you. 
Sign In or Register to comment.