Assy Drawing View Rep

[StephanKlein]

Hi All. I have another newbe question... I made a Simp Rep of an assy for drawing views. I had hoped this rep wouldn't change when hiding parts in the Master Rep. Is there a way of saving a drawing view configuration that won't change unless you modify that rep?
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[eric.mills]

Under your view properties /select view states /and select the rep to be shown in the view.

[StephanKlein]

That is what I've done however, if I go to the 3D model of the assembly and "hide" a part, the drawing part also hides. In other software packages I've used, that configuration is locked and changes to the other configurations will not change it. The only way to hide something in the drawing is to go back to the configuration that was used in the drawing views and make changes there. Is anything like that possible in ProE? This assembly will be used for several drawings and people are always going to be poking around probably messing up released drawings views.

[eric.mills]

There are many ways to control what you want to do. One you could set ready only under the edit menu. You cannot do much with the assy until you clean the read only. Secondly you can convert the drawing view to a draft entity, but now it is a bunch of lines and will never update. Third, use a PDM system to control released objects. Fourth, define you simp rep to such that changes to master will not effect it as you have described. Lastly create a PDF of the released config so that a reference exists.

[StephanKlein]

Ouww Ya! I like number four! How do I do that?

[#6]

Stephan, What I do is set the top level assembly to Def:Exclude Comp. This has worked well with assemblies containing up 200 part/assemblies, more complex assemblies may need other assembly management methods. Select the simp rep, edit>redefine, select the exclude tab, select the top level assembly in the model tree and it should change to Def: Exclude Comp, select the green check mark. Display the simp rep column in the model tree, Display>Add Column. The items to be shown can be set to Master Rep in the Simp Rep column by clicking next to the item name in the column or by redefining the simp rep and using the include tab then select the item. Any new components/assemblies added to the top level will not show in that simp rep until they are set to master rep. When you use hide in assembly mode it will hide that item in drawing mode. Control display with simp rep to avoid this. Use hide for assembly operations and then unhide when finished with your assembly operations. Regards - Chris

[StephanKlein]

< When you use hide in assembly mode it will hide < that item in drawing mode. Control display with < simp rep to avoid this. Use hide for assembly < operations and then unhide when finished with < your assembly operations. Are you saying when you hide a part in the master rep it will still hide that part in the simp rep as well?

[#8]

Yes, that is correct. When we VIEW>VISIBILITY>HIDE an item it "hides" that item in all reps (grayed out in the model tree). Also, if we HIDE an item in a simp rep it will not display in the master rep. This is why we use HIDE as a temporary method of display. For permanent display management of items we will use simplified reps and the items will be INCLUDED or EXCLUDED from the rep. Items we do not want to ever be displayed on a drawing such as construction curves and surfaces we will HIDE. Take a electronics enclosure with a lid for example. With the master rep, while assembling the components inside the enclosure we can HIDE the enclosure lid. When the components are assembled we UNHIDE the enclosure. In our drawing we want to display the enclosure with the external connectors and a view of the components located inside the enclosure. For the interior view of the enclosure we create a simp rep that EXCLUDES the enclosure lid. Hope that helps out. Regards-Chris

[StephanKlein]

So far, it sounds like ProE can't have a drawing view rep that isn't affected by the hide and suppress of the master rep. If someone poking around hides something in the master rep and does a save status, all the released drawings will change???

[#10]

That is right, there is no lock for drawing views that I am aware of. The alarming issue here is that users are allowed to modify released files.