Sketches not updating when parent is changed

[Albigger]

I have had a similar problem before back in R17, (see the bottom of this post for my original thread) but now I am seeing an issue on mulitple workstations with R19:

The problem is that we have multiple part bodies in one catpart, and for instance there is a sketch in one partbody, and a sketch in another body, with a line coincident to the line in the parent sketch. When the parent is updated, the child sketch does not move, even though no errors come up, if you go into the child sketch, the line still shows the coincidence symbol, even though the lines are clearly not overlapping each other. The model IS updated, I have auto update turned on and the "update" icon is greyed out.

If I delete the coincidence constraint in the child sketch, and re-create the sketch, then the line snaps to the new position, but it should do this automatically.

This is very frustrating and could cause a lot of problems in the model if things are not updated when the "master" sketch is updated.

Has anyone seen this behavior before or have suggestions for it? I have seen this on 32bit installs of R19 SP2 with the OS being windows XP pro (both 32 and 64 bit versions).

For reference, this is somewhat of a different issue, but possibly related? Here is my original thread from a while back:

http://www.eng-tips.com/viewthread.cfm?qid=194083&page=1

Thanks.
--Jay

 

[jackk]

In the child sketch, go to Sketch Analysis and make sure the implicit projection to the parent sketch is still valid.

Also, check the Define Work Object is not in the middle of one of the PartBodies.

 

[Albigger]

Everything in sketch analysis seems normal:
under geometry tab, it just says implicit profile, closed, 12 curves
under the use-edges tab, it lists coincidence and offset from implicit projections, and all of them say valid
everything is iso-constrained or under-constrained in the diagnostic tab.

I also made sure the define in work object was not in the middle of a part body.

Still no luck. Thanks for the suggestions though.

 

[Azrael]

Is there a chance that you can strip down the model and upload it?

 

[Albigger]

OK, I have dumbed-down the file and attached it (actually I copied/pasted the two offending bodies to a new part). Rename the attached file from .txt to .catpart

If you go into sketch.20 there are a few lines that are un-defined, where they meet up with the other part body. If you drag those lines slightly, to a new location, and exit the sketch, the other part body does not always update (for me, it might correctly update about 1 in 10 times or so).

Thanks for the help so far.

 

[Albigger]

Anyone try the file and at least confirm they are seeing the same behavior? (Or I'm just crazy?)

 

[Albigger]

Bump.

anyone?

Jackk, Azrael - where'd you go?

 

[PeterGuy]

I cannot get it to go wrong on my R19sp2
Have you upgraded the sketches in R19 (Right click->sketch object->upgrade), or were they created in 19?

 

[jackk]

Sorry, I don't have R19 so can't test your file.

 

[jackk]

Another thought: does it help if you put both sketches into a Geom Set?

 

[Albigger]

PeterGuy - thanks for trying. I don't think they were created in 19, I think 18, but I'm going by memory so I could be wrong. I have upgraded the sketches but it didn't seem to make a difference.

In general, what does the upgrade function do? Are we expected to go thru each feature of our model and upgrade it when we change releases?

Jackk - thanks for looking. I'll see if I can repeat the problem in an earlier version. What are you running? Also, I did copy/paste the parent sketch to a geometric set, and re-linked the child sketch to the parent, and it still had the problem. That is the "normal" modeling method we use (have a parent sketch or feature in a geometric set, with other sketches or features linked to that one within the part bodies).

 

[PeterGuy]

The upgrade changes the sketch to use the R19 sketch which has enhanced behaviours relative to previous releases.

Documentation describes it as below
Upgrading Part and Sketch Features

When improvements or corrections are linked to the update algorithm of a feature, these are always versioned in order to ensure CATIA update upward compatibility. This means that a feature will always be updated using update code linked to the CATIA release version used for its creation.

The Upgrade contextual command available from sketch features, allows you to activate on it and thus access all latest evolutions and improvements available on your current CATIA release.

To upgrade a Sketch feature right-click it and select Upgrade. Upgrade updates all versioning information which is stored in the sketch feature and its content before updating it to take into account all existing improvements and corrections. By the way, this automatic local update on the sketch feature is performed using a dedicated optimized algorithm trying to avoid as much as possible sub-element naming changes in order to minimize the number of reroute operations needed on impacted features when you will update your part data. Nevertheless, upgrade operations can lead to slight changes to geometry. In this case, there is no warning message. Upgrade operations can also require some reroute operations to take full benefit of upgrade operations and retrieve up-to-date part data.
Recommendations

We recommend you:

* Perform upgrade operations on non-deactivated features
* perform upgrade operations on up-to-date features (specially if they contain use-edge features)
* Use Tools > Sketch Analysis before checking its use-edges status and if sketched geometry is solved (solving diagnosis). Due to data modification performed in V5R8, all existing use-edges created before this release cannot be upgraded. We advise you to remove them and create them again. If that is not possible, follow this scenario in order to ensure that the sketch data will be fully upgraded. Otherwise a partial upgrade is just possible and you will not access and take benefit of all available improvements and corrections:

1. Edit your Sketch feature.
2. Select Tools > Sketch Analysis and click the Use-edges tab. You can check whether the sketch contains such type of use-edge data. In this case the Upgrade not possible message appears in the Comment field.
3. Deactivate all old use-edges to fully upgrade your sketch.
4. Exit Sketcher.
5. Upgrade your sketch feature.
6. Edit again you sketch feature.
7. Using Tools > Sketch Analysis activate one by one each deactivated use-edges to see if these use-edges can be supported with the new release version. If not, use-edges have to be deleted and created again.

 

[Azrael]

Just managed to test it on a R19 machine and it's working. Looked at PeterGuys suggestion to upgrade the sketch and it got me thinking... won't a CATDUA do a upgrade on all features in a part?

 

[Albigger]

Did anyone else get a chance to look at this? I'm working on a completely new file now and have the same issue. It's very weird, only 1 line in my master sketch is having the issue (all the other geometry in the master sketch updates just fine). I tried deleting and re-creating this line in the master sketch, no luck. I tried making this line an output feature, no luck.

--Jay

 

[Albigger]

Its almost like CATIA doesn't know the original line moved, so it is forgetting to update the children. I even went into sketch analysis, use edges, and it shows the coincidence as valid, even though you can clearly see in the attached image that it is not coincident.

I have just upgraded to SP4 (was running R19SP2) and the issue still exists.

--Jay

 

[solid7]

Just my $.02 worth...

From what I see, yours is the classic case of trying to do too much with sketches. I know it's not what you wanted to hear, but have you considered rebuilding the part with simplified sketches? (simple lines - no closed shapes)

When I can grab a few moments, I'll send you something. I'm not exactly sure where the problem is with this model -I do see it, but I haven't tried to track it down.

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Catia Design|Catia Design News|Catia V5 blog

 

[Albigger]

Thanks for the help.

So you can confirm the problem, at least?

Unfortunately, I need closed shapes because I need to create 2 shafts with these closed shapes. I was just trying to lay out the outline in one sketch, so when I update it I don't have to remember to update both parts, or I don't have to remember which part is the parent and which is the child, I could just update the master sketch.

The new part I am working on now showed the same behavior. I was able to get around it. Instead of making the line coincidence with the line in the parent sketch, I made both end points coincident with the endpoints in the parent sketch. Now the children sketches update as they should. Still I find this very odd.

 

[solid7]

I did confirm it....

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Catia Design|Catia Design News|Catia V5 blog

 

[Albigger]

This is really getting irritating. Anyone know if this is an R19 bug in general, or is there a service pack that fixes this issue? (SP2 and 4 didn't seem to work)

I'll go for a couple wks without a problem, then it will crop up in a seemingly random CATPart file.

 

[belvedere64]

I don't have R19 to test with, however, I wanted to throw the positioned sketch option out there in case it was something you could use.

/k.c.takacs

/k.c.takacs