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ygupta1-Visitor
1-Visitor
May 18, 2015
Question

Show/Erase Axis Model Annotations

  • May 18, 2015
  • 5 replies
  • 15815 views

Hi Friends,

Can anybody explain me the logic behind "Show Model Annotations" in drawing mode.

I need to do some exercise with Axis in Creo 2.0 drawing mode. I have an assembly having lot of sub-assemblies & parts and when I do select general view in drawing and click on Show model annotations, Only few axis are visible not all.

Now instead of this I have also tried another method by selecting individual part in drawing itself and right click > show model annotation but bad luck.

I have also tried the model tree options as well but doesn't work.

Actually within the same part I am able to see few axis but not able to see which I want to show in drawing. Axis are not hide in model tree or anywhere.

Please come up with your suggestions.

Regards,

Yogesh

5 replies

T
TomD.inPDX17-Peridot
17-Peridot
May 18, 2015

I have had the same problem. I haven't figured out the logic yet, but something about using a different filter when selecting seems to enable selection of the sub-level components axes, dimensions and other annotations.

Y
ygupta1-VisitorAuthor
1-Visitor
May 18, 2015

When I am inserting that particular part (add model) in drawing, It shows all the axis correctly but not for the existing part.

We need to really figure out the problem related to model annotation.

Can we get some PTC expert's suggestion any other idea ???

A
andy21-Visitor
1-Visitor
May 18, 2015

"I have also tried the model tree options as well but doesn't work."

Have you tried looking in the layer tree as well, to check if they aren't hidden there?

layer.png

Y
ygupta1-VisitorAuthor
1-Visitor
May 18, 2015

I have checked, they are not hidden in the Layer tree.

M
MartinHanak24-Ruby III
24-Ruby III
May 18, 2015

Yogesh,

if you can upload the part, then (I hope) you receive and answer very quickly.

Martin Hanak

Y
ygupta1-VisitorAuthor
1-Visitor
May 18, 2015

Martin,

Agreed , I can upload the part but the problem is not only with this part this is a general query as I am getting the same issue with many parts in several drawings.

P
psobejko1-Visitor
1-Visitor
May 18, 2015

Not sure, but is this perhaps something to do with the configuration option show_axes_by_view_scope ?

    Y
    ygupta1-VisitorAuthor
    1-Visitor
    May 18, 2015

    Hi Paul

    I did not find such option in configuration list. Can you please explain in detail ?

    Regards,

    Yogesh

    P
    psobejko1-Visitor
    1-Visitor
    May 18, 2015

    I'm using Creo 2.0.

    Go to the menus: File->Options->Configuration Editor

    You can quickly find options by using the "Find" command - e.g. I look for: axes

    show_axes_by_view_scope.png

    If in your system, this option is set for "top_model_only" then the sub-component axes will not be available for selection by the show/erase tool.

    Try setting it to all_sub_models (which is the default) and see if your problem goes away...

      kdirth
      21-Topaz I
      kdirth21-Topaz I
      21-Topaz I
      May 21, 2015

      If this is an older drawing, the problem may be that the axis have been shown previously and then erased. This leaves the axis in the drawing but hidden and it will not show when using Show Model Annotations. In the drawing tree expand the view datums to see if they are there.

      Capture.JPG

      There is always more to learn.
        M
        mender12-Amethyst
        12-Amethyst
        May 21, 2015

        In relation to erased axes, it's worth noting that if you have a vast number of erased axes that you don't want, generally as a result of having shown all axes in the assembly tree then only kept a few, you can delete them all in batch. To do this, go to the detail options dialog (File>Prepare>Drawing Properties>Detail Options), and issue the detail setup command delete_erased_axes, by entering 'user_command' as the name and 'delete_erased_axes' as the value.

        kdirth
        21-Topaz I
        kdirth21-Topaz I
        21-Topaz I
        May 21, 2015

        I do not see where I can enter the detail setup command. I am using CREO 2.0 and I have opened the detail options by clicking on change.

        There is always more to learn.
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