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S
santinou11-Garnet
11-Garnet
January 16, 2013
Question

Show dimensions by feature and view

  • January 16, 2013
  • 4 replies
  • 22011 views

Is there way to show a dimension by feature and view.

Every time I select a feature on the model tree and do a "show model annotations" dimensions show in some random view.

I don't want to have to move dimensions to the desired view. There used to be an option to "set view current". Can't find it anywhere.

I'm on Creo 2.0.

Any help would be appreciated


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4 replies

T
TomD.inPDX17-Peridot
17-Peridot
January 16, 2013

Great question and yet another fail in the new show/hide incarnation.

Obviously the Model Tree is useless in this regard unless you like moving dimensions from view to view.

I bet the thinking of developers is that since we now we have view highlight from the Drawing Tree (or filter) that we can just pick the dimension we want. Of course, this is often overly optimistic as we may have several dimensions to different features that are identical so picking the specific dimension you want is less intuitive.

What you can do is to use the model tree and pick the feature and in the Show Model Annotation dialog, note the dimension relation value... like d8 for the feature.

Now pick the view in the Drawing Tree (or filter Drawing View to pick the view) that you do want to show the annotation in and go directly to that dimension in the Show Model Annotation dialog and check the Show box for that dimension's "name". Crude, but it works a little easier than moving it later.

S
santinou11-GarnetAuthor
11-Garnet
January 16, 2013

I figured since you can pick a feature on the view itself and show annotations works, why not use the model tree.

Problem with picking a feature from the view itself can take a long time since you have to sift thru many features by way of 'pick from list'- especially if you have a 100 feature model, say--.

Thanks a bunch though. That will have to do

L
linda1-Visitor
1-Visitor
January 16, 2013

choose the feature in the view you want to dimentioning, the related dimensions about that feature show on that particular view and choose the one you want.

i tried it and it works well in Creo 2.0

T
TomD.inPDX17-Peridot
17-Peridot
January 16, 2013

This is correct, Linda. Often, however, it is not as easy as it sounds. I am sure the developers were thinking on the same line. We quickly find work arounds for such shortcomings.

This dialog is nothing like the old show/hide. I still prefer the old method. The new "delete vs erase" is also an interesting implementation than can be frustrating since an erased dimension won't show up again in a different view. You have to remember to delete it or manually move it.

C
Constantin15-Moonstone
15-Moonstone
January 17, 2013

You can select the feature in the 'Model Tree' plus the according view in the 'Drawing Tree' on top using ctrl and then display the desired dimensions.

feature_by_view.jpg

L
linda1-Visitor
1-Visitor
August 14, 2013

choose the view from the screen, and choose the feature from the model tree, and right click and choose show model annotation, see

Untitled.png

creo 2.0 m010

linda

S
santinou11-GarnetAuthor
11-Garnet
June 4, 2014

That does not work Linda. It always shows the dimensions on the very first view added to the drawing. See.. you got lucky by choosing the first view.

I'm on Creo 2.0 M100 and I don't beleive anything will be done about this.

C'est la vie

P
psobejko1-Visitor
1-Visitor
June 4, 2014

Hi Santo,

I'm using Creo2.0 M100.

I am able to select model's feature in the model-tree, right-click on it and select "Show Dimensions by View", after which I pick a drawing view and any of the feature's dimensions that can be placed on that view show up...

I think this does what you want.

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