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sketch fillet, lost relations

sketch fillet, lost relations

sketch fillet, lost relations

is there a setting to retain all your sketch constraints and dimensions while adding a corner-round in a sketch? I'll get really far along, add the fillets, then need to reconstrain and dimension all the sketch entities. I guess it's best to add the fillets as a separate entity after the feature?

RE: sketch fillet, lost relations

Unless the chamfer/fillet have a design impact on your solid, add them as separate entities at the bottom of your model tree.
When it comes to sketches, KISS is the best principle.
Multiple sketches can add flexibility to your design for changes that you do not foresee today.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

RE: sketch fillet, lost relations

Two things to do that can help

One - don't dimension to end points; specifically select the line itself
Two - if that's a problem, as it is sometimes, use centerlines to dimension to and align the geometry to the centerlines.

Centerlines are poorly named as they are only the center sometimes. But I can't think of a better name.

You can also add sketched points at the intersections of the centerlines and dimension to those also. Since centerlines and points cannot be trimmed, the related dimensions can't be lost.

As a further extension for centerline use; never dimension to part geometry or datums if the sketch might be reused. Place a centerline and align that to the part reference and then dimension from that. This will allow saving the sketch with all suitable dimensions in place and ready to re-use. It also insulates if the feature needs to move or the underlying geometry is replaced. All that is required to repair the sketch is to re-align the centerlines to suitable references and no dimensions or associated notes/tolerances/et al will be lost. Saves a lot of time because, done right, any drawing using those dimensions will be minimally affected.

RE: sketch fillet, lost relations

+1 to the above. Re non-centerline centerlines, I think they are called construction lines.


The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: sketch fillet, lost relations

Centerlines are separate from construction lines. I think any geometry can be toggled to be construction, but centerlines are always only centerlines.

RE: sketch fillet, lost relations

These are good tips, the best being KISS. I usually try to add all features in as few sketches as possible. I tend to think like a machinist, each new feature is a new setup.

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