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Show dimensions by feature and view

santinou
10-Marble

Show dimensions by feature and view

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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19 REPLIES 19

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.

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

linda
5-Regular Member
(To:santinou)

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

TomD.inPDX
17-Peridot
(To:linda)

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.

Constantin
13-Aquamarine
(To:TomD.inPDX)

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

I've actually tried doing that and it does not work. It shows all dimensions of the whole model.

That seemed logical to me too and it failed. At least, it failed in Creo 2.0 M030. Do you have a different experience?

So far the best I've been able to do is note the dimension name by picking the feature in the tree and pick it out of the list when selecting the view.

Constantin
13-Aquamarine
(To:TomD.inPDX)

I have to admit that my first enthusiasm got dampened a bit...
It does work, but not every time. It is more like every fifth time. I could not find any kind of rule but if you do it a few time suddenly it works. Then you do the same thing again and the dims show up in several views. Very odd.
Of course this is no solution then. But I think it is intended to work that way which would only seem logic.

my experience has been..if you select a feature in a view it highlights dimensions in that view only in creo 2.0 m010.

This is true but it is not always easy to get at the feature you need.

The original poster is right in that this was much easier in the past with the show/hide dialog.

You are dealing with an -and- condition. So if you click the feature in the tree 1st it highlights where it wants and the view is additive when you pick it in the drawing tree.

This is all I could find from the PTC Support Knowledge Base Search. Lost faith in this one.

show_dim_by_view.jpg

If you can find SPR 1996036, you will see an even more criptic description of the problem. The severity is high and the case is still open. The SPR is linked on that page you posted.

When you translate that to English, it means "Don't hold your breath".

TomU
23-Emerald IV
(To:TomD.inPDX)

The SPR is resolved (closed) as of Creo Parametric 2.0 M060.

TomD.inPDX
17-Peridot
(To:TomU)

Thanks for the update, Tom!

hmmm, this is tech support?

Capture.PNG

linda
5-Regular Member
(To:santinou)

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

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

psobejko
12-Amethyst
(To:santinou)

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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