In-context features of multiple-configuration parts losing definition

[odmullen]

I have a medium-size assembly of piping and tubing components in progress. The tubes are all different configurations of one part; most of them are extruded to length in context. In most cases I mate the tube part base sketch plane and an axis to one fitting, then extrude the single feature "up to vertex" to a vertex on the next fitting in the line. This way, I can move valves or fittings around some and the tube length will update automatically - in theory, and usually in practice. I've had two problems with this, though. First, one time I opened the assembly after a crash snd found some of the tubes extruded in the wrong direction. I added a sketch line on the axis of the tube part and verified that all tubes were oriented properly, so they were all extruding in the same direction with respect to their base sketch plane. I haven't seen that problem recur. THe other BIG problem has occurred twice: I delete a tube from the assembly, whereupon most of the other configurations lose track of the extrude-to feature and I'm left with a whole bunch (40-odd) circles instead of tubes. Needless to say, this doesn't make for a very good drawing of the assembly, and I'm missing another deadline. THe only way I've found to fix the parts is to edit each one in context - over an hour of work last time.
Does anyone have an idea what's causing this and how to avoid it? I could try suppressing tubes I don't want anymore, but I hate to clutter up my assembly.

Thanks for any help..

 

[CorBlimeyLimey]

Afraid I don't know what's causing your problem, but a possible workaround might be to suppress a pipe that you are wanting to delete, do a Ctrl+Q rebuild, resave, & then, if all is well, try deleting & rebuilding the assy.
If it rebuilds OK ... save it quick before it changes it's mind. As a safeguard, make backup copies before attempting major model changes, so if anything goes wrong you won't have to spend hours repairing the model.

Probably the best alternative, if you are doing lots of this type of work, would be to get the Routing package. It's supposed to be quite good.

What version of SW & what SP are you using.
Maybe a long shot, but try a "Repair" of SW. Check faq559-908.

from (the City of) Barrie, Ontario.

If you choke a smurf, what color does it turn?

 

[SBaugh]

Incontexting is very complicated and can make for problems like these to occur.

If your not using routing, and are simply doing this from one pipe with mulitple configs. My question to you is are you in-contexting a single feature to each vertex?Your not allowed to make one feature go to mulitple vertexes without having problems. If you used mulitple extruded features and suppressed the ones that are incontext to a different vertex then things would work better for you.

Not sure if this will help you, but you might want to check out my "Assembly mates and best practices" at my site -

http://www.scottjbaugh.com/Tips_Tricks/Tips_Tricks.htm

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[TheTick]

I recommend putting another "layer of definition" between the in-context definition and the extrusion.

Since you are extruding "up to vertex" in-context, perhaps try this approach:

•From the assembly, while editing the part, create a 3-D sketch. Sketch a point and make it coincident with the vertex of interest.
•In your part, define your extrusion as "up to vertex" using the sketched point as the vertex reference. NOTE: sketch points can be used as vertex in SW2003 and later.

This approach will be more robust. The reason for this is that if there is trouble resolving the in-context sketch point, the point will at least still be drawn in its last known position, and the extrusion will still resolve its end condition at that point.

An alternative to creating points in-context may be to create planes in-context and extrude "up to surface".

Due to illness, the part of The Tick will be played by... The Tick.

http://www.EsoxRepublic.com

 

[odmullen]

Thanks for the thoughts, all. I suspect that Scott's insight is most accurate, although I am curious as to where in the SW documentation it is stated that extruding one feature go to mulitple vertexes in different configurations will cause problems. The odd thing is that it works for days at a time, thru crashes, saves, rebuilds and reboots, deletions and additions of configuration instances and modifications of the context geometry, then suddenly it fails. Even more odd is that after repairing a few of the tubes, a bunch of the others remembered their definitions and repaired themselves. Evidently the capability to do what I'm doing is there, but isn't perfectly robust - somewhat like "parallel" mates that forget their orientation and turn up reversed once in awhile.

Tick's idea of 3-d sketches or planes appears to have ther merit of greater stability, but I suspect it begs the question to a degree - if the software loses track of the extrude-to feature in context it might very well lose track of the association between a plane or point and the same feature. The advantage of having the feature persist in such an event is dubious - a cut list of parts that are not properly associated with the context will cost more than a cut list of a bunch of tubes of "0" length.

I'll try the multiple-feature approach at the next opportunity and see if that is any more stable. It's only happened a couple of times, so frequency statistics are going to be a little shaky...

 

[SBaugh]

Well If you do and "up to vertex" or "Surface" on a single feature. How would SW be able to distinguish between this vertex and that vertex?

I just tried a small example using the same pipe with one feature and two separate assembly planes. And when I edit the Feature and change the "Blind" to "Up to surface" it works for Plane 1. When I add the same pipe to the same assembly and Re-edit the same feature and tell it to extrude to plane 2. It does it. But now (I mated the Pipes together Coincident and concentric) the first pipe intersects the second pipe.

I have an example at my site.

http://www.scottjbaugh.com/Design_Portfolio/Incontexted-Steel.zip

1) Unsuppress everything in both the assembly and the parts
2) Change the location of Plane 6 and the length of Tube1

Tube2 will follow Tube1 and changing Plane 6 will cause Tube3 to follow.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[SBaugh]

I also have this example.

http://www.scottjbaugh.com/Design_Portfolio/VBAExcelExample.zip

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[odmullen]

Scott
It seems that the target vertices are unique entities that should be reliably associated with each tube configuration. Each configuration is extruded to a different vertex in the assembly (however, they are sometimes vertices on different instances of the same part). I would surmise that the extrusion length is determined by calculating the distance from the referenced point to the base sketch plane, just as would be the case if it were extruding to a sketch point, a plane, a surface, or the end of a line. The software apparently does keep track of the definitions and vertex locations, but occasionally forgets where it put the info and throws up its hands until the user provides enough clues to restore the associations. I was pleasantly surprised that it self-repaired most of the tubes this time. Last time it happened I had to fix pretty well all of them, and doing the same thing to 50-odd parts is really boring.

Having a different extrude feature for each configuration may be a good workaround, but it would be better yet if SW could figure out the root cause of the instability and fix it.

 

[SBaugh]

I don't believe it to be an instablity. I believe it to be a limitation with no workaround, then what is already out there.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[odmullen]

OK. Call it sporadic functionality, then.

 

[ShaggyPE]

Rather than using configurations, you could use different parts. Then the up to vertex or surface will have no problems. The only draw back here is, now you have multiple part files.

 

[SBaugh]

That's why I suggested having the multi-feature part file with Configs. That takes out the issue of multiple files. Either way would work.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376