second issue of the day. I have recently started working with family tables & so, do not have much experience with them. I am having no problem creating them, varying dimensions, excluding features etc, creating the resultant drawings, but i am running into problems if a want to save a copy of everything created. Let me explain, i have a part 'a' with an instance 'b', i have a drawing for each part also named 'a' & 'b'. Now, when i save a copy with new names, i get both parts but only one drawing, plus the parts have become independent of one another. So, what i get appears to be the following, i save as, part 'a' to part 'c', i get part 'c' with drawing 'c', but i'm not getting instance 'd' with a drawing 'd', i still have instance 'b' with no associated drawing, plus when i look at my new part 'c' there is no longer any family table. I hope this makes sense to one if not all of you.
Thank you in advance
If you have Intralink or PDMLink, this should be possible. If not, it might be easiest to copy all your files into a new folder, open these in Pro/ENGINEER and rename, then you should be able to move them back to the original folder without conflict.
Thank you for the info Andrew, we do not have intralink so copying the files as you describe may be my only option, but renaming everything each time will be a pain.
"Rename in session" is also a powerful tool to create copies.
Open all the files that you want to copy (parts and drawings), then rename each one to the new name, remembering to select "Rename in session" each time.
Then save everything, first making sure that you're in the correct working directory.
I haven't tried creating separate drawings of family table instances - here, we only create drawings of the generic, and show a table of the instances, and this approach works as you'd normally expect - so I don't know what other quirks you might find.
Thank you very much, that worked a treat, the only problem i had was saving all my renamed parts & drawings to my working directory, using save i found that pro-e would only allow me to save my new parts & drawings in the directory from where they were originally sourced, but 'back up' did the trick.
I have a suggestion for a the drawing.
If your drawing is not very complicated, you might also be able to use one drawing for all possible instances. In drawing, go to the "Drawing Models" and use "Set Model" option to set a different instance as your active one. This way, you can use one drawing (as a template) for all sizes (instances). I had used this option very effectively, but will get complicated if the drawing is not simple as it would be difficult to control the placements of the dims / notes. To a certain extend you can use snap lines to do that but still...
The advantage is not only in creation of the individual tiff drawing but also is in the modification.
Can be useful in some cases.. see if its applicable for you.
your suggestion was indeed useful. I am creating muti-sheet drawings all the time, & adding & setting models in the way that you described, but it never occurred to me to use this technique here. I am now able to "save a copy" to create a new part with new instances, i just have to rename my new instance as it comes across with the old instance name.
dear thanks for reply,
i want to add in bom table like
all parts name, qty, material, description & all things necessory for bom.