How to hide part's datums of subassembly in main assembly?

For example I have one subassembly with three parts and I'm placing it to
main assembly and I'd like to see only main datums of this subassembly but I
see also datums of all these three parts.
Wildfire 2

 

If you have a layer in your part that has the datum's on, you can go to
the layer tree in the part, hide the layer with the parts on,
right-click & save status. Then save the part - this will hide all of
the datum's in the part for the assembly as well as the part itself.

 

It would be fine, bu I've just found this notice in Hepl:

"The hidden status of items is session-dependent; it is not saved with the
model. All hidden items are redisplayed automatically when you exit
Pro/ENGINEER."

But I Thank, it's helped me a bit.

 

I'm using this in Wildfire 2.0 M020 and M080, and by saving the
status and saving the part, it doers keep the datum's hidden from one
session to the next.

 

Hidden status only refers to those items in the model window or tree
upon which you right-click and select 'Hide'. The Help notice you read
is not referring to layer display statuses. If you change the layer
display, do a 'Save Status' and then save the file, in the next session
the object will reload with that layer status.

Regards

 

For example I have one subassembly with three parts and I'm placing it to

In the Model tree, RMB the features, Hide or Unhide as desired. (Hide can
be done in the graphics area.)

If you wish to make the change persistant, RMB the component, Open, Save
Status (be one of a few methods), Save and Close.

 

Many Thanks to all for useful suggestions.

 

I'm using WF 2.0 M030. Is any switch in config.pro, which allow to save
automaticaly display status during normal save? In this moment, I'm saving a
part and a display status separately (File -> Save; View -> Visibility ->
Save Status).
Thanks in advance

 

I'm using WF 2.0 M030. Is any switch in config.pro,

I don't believe it's possible.

You must Save Status to make the Hidden status persistant.

There are two factors to contend with when working in an assembly. Saving
the layer status and then making sure the part is saved to disk.

When working in an assembly, if you have made a change to the part that
will cause it to be saved when you save the assembly you'll be good to go.
If you have not (the only change to the part was feature visibility) you
must explicitly save that part, otherwise the part's saved layer status
isn't saved to disk*.

You might want to make mapkeys cut down on the mouse work (that's my
preference). You can also use the Select option in the File Save dialog to
pick and forcibly save individual part files while in the assembly

http://www.mcadcentral.com/proe/forum/forum_posts.asp?TID=27046&PN=3

is another discussion where I asked the same question. (*There's mention
of a config option that causes all files to be save when the assy file is
saved. Not a good deal, IMO, though.)

Let's see what else might come up here.