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garytinker1-Visitor
1-Visitor
June 17, 2013
Question

section views in family tables

  • June 17, 2013
  • 4 replies
  • 7051 views

Hi guys and girls,

 

I’m having a real drama with creo today, something that worked in wf5 but apparently not in creo 2.0

 

Here’s the beef,

i have a family table assembly in side of that family table are multiple variations of a product

There all rectangular, all the same size and all have the same mass

What’s different is that there are different positions for steel boss's or holes or whatever in a sub assembly of the main assembly

 

somthing like this

 

main asm name sub asm 1 sub asm 2
parent asm parent part 1 parent part 2
child asm 1 part 1 vers 1 part 2 vers 1
child asm 2 part 1 vers 2 part 2 vers 2
child asm 3 part 1 vers 3 part 2 vers 3

where sub asm1 and sub asm2 are inside main asm

 

  • So when i go to make different drawings of each of the family table children i need x sections
  • So in the master assembly in the family table i put the sections in.
  • Open a child assembly in a drawing file, no sections also no sections in the child asm file,

 

So then i think,

Make x sections in the child assemblies then they will show up

 

This works kind of.... i can open the sections in the drawing files for each child assembly, great save

Next time i open the file they have all disappeared from the child drawing and the child assembly

They have shown up in the parent assembly but there all supressed and i can’t resume them.

 

This is got me stumped. How do i go about making x sections now? Am i just missing something?

 

What I think is happening is that the section is not finding the part it sectioned in the master file in the child file so it suppresses its self rather than re calculating for the current child assembly?

 

i can make sectons in the child drawings if all versions are exactly the same so the section plane does not cross or reference anything that changes between child and parent asm

 

Any help would be great

 

Cheers Tinker

 

also sorry if this is a ramble


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4 replies

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TomD.inPDX17-Peridot
17-Peridot
June 17, 2013

Yet another compelling reason not to use family tables

I looked through the open and resolved issues for Creo 2.0 and didn't see anything along these lines.

If you can make this a coherent case for customer support, it would be good to submit. The fact that it works in WF5 and not in Creo is a strong argument for the problem being the code, and not the "grayware".

What version are you on? And can you post more info; images or even simplified files that exhibit this problem?

In theory, you should only have to make the section in the assembly you display in the view. Creo has been plagued with cross section issues since ... well... pro/engineer. But something really bad seems to have happened to the code because it has become quite unstable by missing complete surfaces and failing to outline section edges. Adding family table issues is not something that's been mentioned a lot. Maybe you uncovered a new bug that really should get in front of PTC engineers.

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garytinker1-VisitorAuthor
1-Visitor
June 17, 2013

Heh, family tables drive my up the wall but if there was another way to do what we need to do that was "usually" as easy- then we would do that....maybe there is?

I’m running the latest distro of creo parametric 2.0 currently, last time i made this work was the pro/e creo x over version of wf5

cant really show what I’m working on, cut throat industry and ip is stolen all the time, but I’ll see if i can knock something together tonight that gives a example....

ive been thinking that i have found a ibkac error but you give me hope that it’s not the case

B
BrianMartin13-Aquamarine
13-Aquamarine
June 17, 2013

Hi Gary...

Do you have anything you can share with us in terms of Creo files? You should be able to add the cross section in the generic and then show it just fine in the drawing. If this isn't working, there's a few things you might try.

First... make a drawing with all general views (all generics). Show the cross sections you want... and then replace the models in the drawing with the correct instances. See if the cross sections stay or not. They should.

This is one of those things that might be easier to diagnose and troubleshoot if we had some sample files to play with. One other thing to try would be Creo 2 M060 which was just released. Maybe this is just a problem with your version of Creo?

Thanks!

-Brian

A
adept3-Newcomer
3-Newcomer
October 27, 2014

Was there ever any resolution on this issue? We just ran square into it! With problems like these how can PTC still promote their methods relative to family tables. I use them but hate them. Being a user since Rev 4 (most of you never heard of that)

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garytinker1-VisitorAuthor
1-Visitor
October 28, 2014

i havnt realy found one,

the only thing i have found that works is a pain in the ass

basicly you have one section for each child and make sure that the section only gos through the features that are turned on in that child. if it crosses an area that has turned off parts it will fail.

its a pain because you have a drawing that has section f-f but no section a-a through e-e

and this only works some of the time, the next time you open the project the section might be supressed in all children

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adept3-Newcomer
3-Newcomer
October 28, 2014

What I found out was what I tried initially but it didn't work, so I called the hotline. I haven't run with this much but theoretically it should work and I have tested it. Any section that you want in all instances must be created in the Generic and just like Gary said, a section is just like a reegular feature, if you supress any parent of that section in an instance then the sction will supress with it. So, from a drawing perspective PTC (who usually respects drawing practices) requires your sections to be Generic and not from model geometry (if you want to be safe). Of course if you don't care if you have section letters in your drawings not being sequential and haveing downstream departments reading drawings and saying, "her's section B and here's F, where's C,D and E????, we must be missing a sheet!?" So, making sections actual features may not have been such a great call, however, I have noticed some increase functonality as it relates to sections, but, drawings be dambed! I guess the coders and decision makers think everything gets made with desktop pronters or something and the drawing is dead? but I won't rant. I hope this helps...

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ptc-30508101-Visitor
1-Visitor
January 22, 2015

Hi Gray,

I am also facing the same issue that you are. But finally i found the solution...Its very simple. As you describe once you close all the drawing and generic model and again reopen the drawing its missing and you got error. After that I have open the instant model and check the cross section in View manager its on Resume model, so all ok, after that i have check this in generic model its suppress so i have done edit defination for this, ask for reume section, click OK and its resume then save the generic model and close all window. Again open the drawing and it works!!!

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TomD.inPDX17-Peridot
17-Peridot
January 22, 2015

Welcome to the forum, Kamlesh.

The idea of having to track down regeneration errors on opening a drawing is simply not acceptable.

I know we discuss a lot of Pro|WorkArounds^tm here in the community but at some point, we have to call it what it is... a bug. I have a few models that I created with all due diligence that once opened in a drawing from a clean memory state, always have regen errors at some errant location in a sub-component. However, when I open each part and then open the drawing, no problem. Again, this is simply unacceptable.

If you have a good example that you are willing to share with customer support (if you have maintenance), I would love to hear PTC's response to these types of errors.

As for a use case where this is unacceptable; all too often drawings are generated without any operator to confirm their accuracy. A program calls up the drawing and outputs a PDF during offline hours. That output should be absolutely correct to the original intent!

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