Single sketch for two close tolerance mating parts

Isoworks

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.

S1mon

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.

Isoworks

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. 

wayne_sauder

  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. 
 

mahir

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