I have modeled complete product using top down design modelling approach. Skeleton is used to define the internal size of product and complete model is build with reference to this skeleton. This product have approx 31 variances based on its internal size. There are some of the parts/components/features which are required only for particular model, the visibility of such parts/components/features in assembly model was controlled using program and relations. Now the model is almost complete and I have noticed following issues:
1. Suppose there are 1, 2, 3, 4.....31 variance and in which 1a, 1b, 1c are some of the parts which are required only for variant 1. Whenever I changed the skeleton model dimension to variant 2 and then try to open the part/drawing file of 1a, 1b, 1c regeneration error was observed.It shows the missing references even though all the reference were defined with reference to assembly references during modelling. Need help to avoid this regeneration error or tips to define the references.
2. Suppose there are 1, 2, 3, 4.....31 variance and in which a, b, c are some of the parts which are required only for variant 1 to 5 and d,e,f are the parts which are required only for variant 6 to 10. In this case whenever I set the skeleton model dimension for any variant between 1 to 5, part/drawing file of d, e, f also get re-sized even though this part file is get suppressed when model variant is between 1 to 5 and vice versa in case when model variant size is between 6 to 10. How to avoid the re-sizing of part file when it is not required in active assembly model file.
Request all to help.
Thanks & Regards.
Thank you for explaining this so well. This is a very serious undertaking.
I think you broke the software ...Just kidding.
Because of the high level of involvement, I am 1st going to suggest creating a support case and having tech support zero in on the issue by reviewing the file.
This is why we pay maintenance, and it can only make you smarter, or the software better.
Having said that, regeneration processes are touchy. I know that some regenerations fail in exploded state assemblies due to mating conditions. Regenerations also fail due to hole changes where a different hole definition is taking place due to some intervention that might be taking place in programming. Holes that change type are assigned new internal IDs. This might be happening to surface in some instances as well.
This really comes down to a case by case basis. It is extremely frustrating to get this far into something only to have it fail for obscure reasons.
To get the help from the community, you may need to share the file and the conditions under which it fails specifically. Again, this is why I suggest working with tech support. They are chartered to get to the bottom of this, and if they fail to, you escalate the case. Your use case is what PTC says their software does better than anyone else.
Thanks Mr. Antonius Dirriwachter for responding on my queries.
As the assembly model I have created is quite big, I have attached the image and model files for sample case of top down modelling where similar problems observed. In this case there are two parts PART1 & PART2 which are controlled/referenced by skeleton dimensions d0:280 & d1:280.
In this case as PART1 is suppressed I found the regeneration error when I opened that part file. The regeneration errors are not due to assembly constraint but its due to missing references used during extrude definition. Pls go through the model files and It would be grateful if you can help.
As you suggested I have also contacted PTC India support and asked for their help.
your part1 contains geometry referencing the assembly aa1, the sketch of the extrude uses two curves from the skeleton.
Hence the sketcher geometry inside the part depends on the skeleton geometry, but also on the placement of part1 and the skeleton (the relative orientation between both makes a difference)
The problem in your example is, that the part currently is not in the assembly (it is suppressed) - hence regeneration fails when it tries to fetch the references for the update.
To make full use of the skeleton functionality (and to solve your issue), you should not reference geometry directly (like in sketcher).
Create a copy geometry feature in the part and copy all geometry you need from the skeleton:
Under the Options of the Copy Geometry feature, you find the section Copy geometry Update, which allows you to decide when you want it to update (and as long as the part is not in the assembly it is no good time to do it).
If you set it to No Dependency it will stay as is and never care of the assembly - if you want it to update you can later change the setting again.
The sketch can then reference the curves in the Copy Geometry feature.
Your instructions really work for me to some extent. I have following assumptions/doubts as I started working on your instructions:
Only few questions for a moment, will come up with few more as I progress.
Pls keep replying.
Sorry for being late with replies:
1. that's right, some steps to be done, but changing afterwards is always more time consuming than doing it i first place
2. That's the price you have to pay for the flexibility to switch updating on and off. The shortcut compared to copying the needed geometries one-by-one at the target level, is to use the Publish Geom feature in the source part (skeleton). This feature will be defined with all geometry that should be copied. It works as a container. Then you only need to select the Publish geom feature for copying into the other parts and have all geometry available.
3. you first need to checkmark Dependend again in the feature
If there are missing reference reported then you need to set "Search_Path" option your config option to the locate the right folder in your local drive..