Problem with SW2008 Reference dimensions

[Jasonx10]

Im having a nasty time getting my reference dims to stay when i place them in my main assembly ('tis getting rather large in size; 8000kb or so). Let me explain-

The goal here is to simply plop a few dims into my assembly and run off a few tabloid size prints for a customer (its a room layout and he's looking to see distances from floor to pipes and other such goodies).

I go to select surface to surface or whatever, it shows me the dimension - i try to place it and *poof*, it vanishes on me (every time without fail).

I thought perhaps it was my display options (and suspect that it still may be).

The only way I can get these dims to show up at all is to display 'all annotations' (under 'view'); which - inconveniently enough - also turns on a bunch of other annotations hiding in several sub-assemblies.

I feel as though I've tried everything to no avail and am growing closer to tearing several of my hairs out.

Certainly there must be something I have missed? Any ideas here?

Thanks
Jay

 

[MadMango]

Try creating a drawing of your assembly and placing your dimensions. It sounds as though you are just dimensioning the assembly it self and printing that.

"Art without engineering is dreaming; Engineering without art is calculating."

Have you read faq731-376 to make the best use of these Forums?

 

[Jasonx10]

Yes. I was trying to just print a picture of the model with dims showing (without necessarily throwing it into a drawing). I don't know for sure that I've ever tried it before; I thought I remembered being able to do this in past versions of SW, but i could be mistaken here.

I know it lets me pull the dims off - i just can't find a way to display them without hitting the display 'all annotations'.

 

[JMirisola]

If you use the smart dimension tool (in the sketch toolbar), you should be able to create your dims without them disappearing.

Jeff Mirisola, CSWP, Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

 

[CorBlimeyLimey]

Do you have the Enable Annotation View Visibility option selected? (RMB on Annotation folder)

Are you pre-selecting or creating an annotation view for the dimensions to be placed into?

Do you have the Automatically Place into Annotation View option selected?

 

[Jasonx10]

- yep

- yes

- yes also

Double checked my display filter under tools, options, document properties, annotations display also and I have feature, reference and dimxpert dimensions all checked. Display assembly annotations below is checked also.

For some reason, the ref-dim shows up when i select surfaces, but the moment I go to drop it, it vanishes unless (and this is the only exception so far) I change my view options to display all annotations.

 

[CorBlimeyLimey]

Which graphics card and driver are you using?

 

[Jasonx10]

ATI FireGL 7200

Downloaded the newest driver for it for SW2008 off SW website not but a few weeks ago even.

I havent really had any graphics issues though (unless this turns out to be my first).

I suppose it could be some kind of fluke - I just feel like I've got to be missing something in my settings though; just not sure what it is.

 

[JMirisola]

Did you uninstall the old drivers before installing the new ones? If not, you should.

Jeff Mirisola, CSWP, Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

 

[Jasonx10]

hmm...nope! I will try this. Thanks.

Jay W.

 

[handleman]

Sounds like proper behavior to me. There are two aspects to annotation visibility - the "View" menu and the "Annotations" folder in the feature tree. View->All Annotations chooses whether or not to hide (not really show) all annotations at the current document level and all lower levels (subassemblies). Real annotation visibility is set in the document owning the annotation and "bleeds" up from there. Setting the Annotation Visibility in Tools->Options Document Properties tab has the same effect as right-clicking the Annotations folder in the feature tree. If "Show Feature Dimensions" is checked in that right-click menu for a part, then any assembly containing that part will display the feature dimensions of that part unless "View->All Annotations" is deselected in the assembly.

To get the behavior you want, you will need to:

1. Enable View->All Annotations in your main assembly.
2. Un-check "Feature Dimensions" and "DimXpert" dimensions in Tools->Options Document Properties or by right-clicking annotations folder in the feature tree in your main assembly. Make sure "Reference Dimensions" is still checked.
3. Open each part or subassembly that has dimensions "bleeding up" into your main assembly and un-check any annotation types that are checked.

-handleman, CSWP (The new, easy test)

 

[CorBlimeyLimey]

Although the ATI FireGL's are supposed to be OK for SW, some people still have problems, especially with the 7200.

If a clean re-install of the SW certified driver does not fix the problem, try the latest one from the ATI site.

Do you have accaess to an nVidia Quadro (not NVS) card to test?