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bobjohnson351-Visitor
1-Visitor
July 13, 2017
Solved

Unable to access set datum tag in creo 4

  • July 13, 2017
  • 27 replies
  • 18329 views

Can someone please explain to me how you are supposed to set the placement of a datum in creo 4. The "set datum tag" no longer includes the option for placement when you select properties.

 

This explanation might as well be in greek for all it means to me:

 

"Change in product specification with Creo Parametric 4.0 F000

  • The annotations in the model would better adhere to the GD&T standards (both ASME and ISO) and capture the full semantic intent"

https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS260600&posno=1&q=260600&source=search

 

I want to be able to do this:

http://www.ptc.com/cs/help/creo_hc/creo20_hc/index.jspx?id=To_Set_Datum_Plane_of_a_Model&action=show

Best answer by StephenW

That link led me to a nice little video of how it magically works.

https://www.youtube.com/watch?v=yULd7Dl5fcA&feature=youtu.be

 

EDIT: that was in this blog https://community.ptc.com/t5/Creo-Blog/Did-You-Know-Enhanced-Datum-Feature-Symbols-Available-in-Creo-4/ba-p/444159

which also contains a link to PTC help that links to non-linear x-hatching????

27 replies

StephenW
StephenW23-Emerald III
23-Emerald III
July 14, 2017

I'm not on Creo 4 yet so I'm not much help.

The CS document you linked to also had an SPR associated with it. Usually that means there is a bug.

T
TomD.inPDX17-Peridot
17-Peridot
July 14, 2017

Not sure as to the specifics of your question.

It appears the functionality was eroniously removed.

That wouldn't be the 1st time they did that to see the response.

If no one complains, it is obviously not required.

Anyway, that is what I am seeing way to much of in going past Creo 2.0.

Similar problem from Pro|E to WF... WF to Creo...

Seems PTC is just weighing their "liability" and quietly removing features.

 

I once reported a problem by not being able to select a datum point.

The little black dot got in the way of the actual feature and you could not select the actual point.

The Pro|WorkAround(tm) was to turn on the datum tags which were selectable.

This bit of info is only useful if you are just having trouble selecting the datum.

 

Did you submit a support case for this question?

It will be interesting to see PTC's response.

 

B
bobjohnson351-VisitorAuthor
1-Visitor
July 14, 2017

Yes i logged a support case. I haven't heard anything useful back so far from PTC. I don't understand why they would have removed this feature. All im trying to do is attach a datum flag to a diametral dimension or an existing geometric tolerance. I must be missing something basic....

StephenW
StephenW23-Emerald III
23-Emerald III
July 14, 2017

I haven't taken the opportunity to get on 4.0, here's the screen shot of creo 3 datum in the draiwng and in the model. What does the creo 4 - right click properties look like in the drawing and in the model?

datum-attach.jpg

 

datum-model.jpg

D
dschenken1-Visitor
1-Visitor
July 14, 2017

I don't see it now, but there was a post to the effect that PTC was changing how the placement system was reworked to prevent users from adding datum feature symbols to axes because that is prohibited. It seems like the post also alluded to some other placement functions that would also not work, but would be re-enabled in the future. Over in the Creo Blog there's a post that indicated they have been busy on the MBD side of things. https://community.ptc.com/t5/Creo-Blog/bg-p/CreoBlog

StephenW
StephenW23-Emerald IIIAnswer
23-Emerald III
July 14, 2017

That link led me to a nice little video of how it magically works.

https://www.youtube.com/watch?v=yULd7Dl5fcA&feature=youtu.be

 

EDIT: that was in this blog https://community.ptc.com/t5/Creo-Blog/Did-You-Know-Enhanced-Datum-Feature-Symbols-Available-in-Creo-4/ba-p/444159

which also contains a link to PTC help that links to non-linear x-hatching????

    B
    bobjohnson351-VisitorAuthor
    1-Visitor
    July 14, 2017

    Stephen,

    Thanks for the link to the video - thats exactly what i was looking for (not sure why PTC support wasn't able to just point me to this...). It looks like they have moved to MBD for creating gtol datums and attachments as annotations. 

     

    This what the datum properties menu in drawing mode in creo 4 looks like:

     

     

    B
    Bogdan1-Visitor
    1-Visitor
    October 22, 2018

    I have updated to using CREO 4.0 M060 and now you can create the datums in the model also and bring them to the drawing. Datum A was created in the drawing and doesn't have a feature in the model. Datum B and C were created in the model and bring them on the drawing view. In the drawing tree, you see the datums are in different "groups", the one created in the drawing is seen as a draft and shown in the Annotations group and the ones from the model are in Datums group.

    2018-10-22_8-02-31.png2018-10-22_8-03-01.png

      G
      GaryLinscheid15-Moonstone
      15-Moonstone
      October 22, 2018

      Set the config.pro option default_gtol_owned_by_model to yes

        Chris3
        Chris321-Topaz I
        21-Topaz I
        October 22, 2018

        Add the config that @GaryLinscheid said but also - don't create feature datum symbols in the drawing. They are not parametric to the GTOLs. Also use the datum feature symbol icon in the annotate tab of the ribbon. Don't use set datums defined by datum planes anymore. PTC has changed the workflow to better mesh with model based definition (MBD). Embrace the change now even if you are not using MBD and save yourself headaches later on down the road.

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