incontext relations and fillets

SW2004/SP1.0
The incontext sketch relationships between parts (b, c, d) are broken
whenever I edit the fillet on reference part (a). This has happened more
than once this past week (same assembly). In this particular case I have
been editing parts (b, c, d) in the assembly and applying sketch offset and
cut extrude.
Each time I make a change to the fillet it creates errors in the assembly,
parts and or course dangling dimensions in the drawings. Not fun or
productive
Possible work around: make my mind up and stop editing the part fillet size
Kman
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Kman
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I'm sure we'd all be interested in whether SP2.1 makes any difference.
Kman wrote:
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Sporkman
Is this a known issue?
Kman
Reply to
Kman
I have found that it is better NOT to make incontext relationships to part features (eg. faces, edges, etc) as they are prone to 'going walkabout' when you edit then or add fillets & chamfers, etc, instead I show the sketch that created the feature and make the relationship to it - much more robust - very rarely have an assembly with cherries in it now.
Merry :-)
Reply to
Merry Owen
I have read many of your helpful and practical posts in the past and recall the "creating relationships to sketches, planes etc.. as opposed to picking part features and surfaces." I have used feature sketches for dimensioning though obviously not consistently. Will give this a go and see if it reduces my frustration level.
Thanks, Kman
Reply to
Kman
We've been having similar problems with cherries showing up in other parts after changes, probably due to in-context relations, and the SP (0, 1 or 2.1) doesn't seem to make much difference, although we haven't done enough on 2.1 to know for sure. Merry's more robust design methods do seem to help; I was able to fix one of the persistent problems.
Jerry Steiger Tripod Data Systems
Reply to
Jerry Steiger
With each passing project I am shying away more and more from in-context design. I generally work on plastic or cast parts, and for this, I way prefer doing multibodies with the split part function. I model the assembly as a single part, making all the important geometrical relations in the part file, then split it up into individual parts and put it back together as an assembly.
In plastic parts, draft and fillets would get you in a lot of trouble with the non-history based incontext features. You would only be able to make relations to sketches, planes or finished parts.
There was a thread a while back disparaging the split function, and I do admit it is not for the faint of heart, but this avoids most of the downfalls with in-context, including the configurations caveat.
I know this way of doing things might not work well for sheetmetal design or machine design, but for what I do, I think its great.
matt
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matt

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