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.

Options

Single sketch for two close tolerance mating parts

IsoworksIsoworks Member Posts: 22 PRO
Hello,

What is the best process for sketching two parts - a hole and a shaft - that have a close tolerance fit? Do you really draw two circles basically on top of each other? 

I have modeled a number of parts in a sketch that are line to line. This is great in the sketcher but it creates part fit issues upon review for manufacturing. 

There must be a better way to address this.

Comments

  • Options
    S1monS1mon Member Posts: 2,412 PRO
    I always model in clearances, and I always like to model things at nominal with symmetric tolerances. This is considered best practice for 6 Sigma. Asymmetric tolerances are ok if someone is making a small number of something and an educated machinist is trying to creep up on a fit, but for mass production, it's not usually preferred. 

    So, yes, I will often do this with two circles that are slightly different diameters. In Solidworks I was inclined to draw the shaft with a solid line and the hole with dashed lines. Depending on the situation I would dimension the shaft or the hole and then the clearance between them, but in other cases I can see wanting to dimension each diameter independently.

    For some types of complex clearances, I will use move face or even boolean with an offset.
  • Options
    IsoworksIsoworks Member Posts: 22 PRO
    I understand. 
    However, it seems like this should be a feature that exists in the extrude or revolve function. I would just like to see a better process flow around something that is so common. 
  • Options
    wayne_sauderwayne_sauder Member, csevp Posts: 484 PRO
      I have spent a good bit of time trying to figure out a good workflow for this. My preferred method right now is to use offset in a sketch, that way it changes if I change the main geometry. One thing that I need to remember to do more often with this is to use a variable to drive the offset (easier to change multiple offsets in a project quickly). 
      @Isoworks what are your thoughts on a better process? I would vote on an improvement request if someone submits a good idea. 
     
  • Options
    mahirmahir Member, Developers Posts: 1,292 ✭✭✭✭✭
    This is one of those things that comes down to preference and/or specific process/application. The options that come to mind are:
    • Separate sketch elements at nominal (as @S1mon suggested)
    • Separate sketch elements at max (MMC) or min (LMC) material condition
    • Single sketch element and line-to-line parts with clearances called out in drawing/MBD
    • Single sketch element with offset surface after the fact, usually to show MMC
    I personally prefer the last one. Then, in the drawing I'll use either one-sided tolerances or a range. The offset can be adjusted to use symmetric tolerances, depending on the manufacturing method and functional fit you're trying to achieve. The offset method has several notable benefits.
    • Your sketch can stay simple, avoiding almost-overlapping sketch entities which I personally find annoying to work with
    • The offset is a separate feature that's easy to adjust independent of the main sketch
    • The clearance is still controlled in the model vs the dwg
    • Great for tweaking clearances of 3D printed parts
Sign In or Register to comment.