Exporting and importing draft groups in Creo Parametric (drawing)

[Mat]

Hi there,

I am looking for a way to save a draft group to a file and importing it later to another drawing.

Background:

I try to define a drawing note according to ISO 22081. Works fine so far.

I use a draft group, which consists of a common drawing note and a geometric tolerance dimension

Please let me know how to export and import the draft group or if there is a better way to get the ISO 22081 note to a drawing.

[StephenW]

You can't do it with a draft group

You can use what you have and create it as a symbol to  be re-used.

I do something similar for "old drawings" that get converted to the new drawing format but I need to keep the old "standard" tolerances.

[Mat]

Thanks for Your reply.

I was afraid that saving draft groups just is not possible.

I tried converting the draft group to a symbol, but unfortunately I lose the ability to modify the dimensions.

But the "edit symbol" - interface is quite ancient and I am not very used to it. So maybe I am missing something.

[StephenW]

"Ancient" may not be a strong enough description 😁 

You can make your text variable so you are allowed to change it.

For the GD&T, I think you will have to use "text" instead of a dimension. If you are using creo 4 & up (I think it started on 4) you can use the "box" text to get it to look right. Turn "box" on and off to show the split lines between each. Make sure your value and datums are variable so you can adjust as necessary. 

I'm on Creo 6 so your menus may vary some depending on your software version.

[pausob]

I assume this draft group is already part of your "standard drawing template" and this is for updating legacy drawings?

I suggest making a simple drawing "iso22081_note.drw" (no models and no formats) with your ISO22081 note as a draft group as the only content.  Then import that "iso22081_note.drw" into your new drawing.  That import could be automated via a mapkey assigned to a button.

The draft group will show up on a new sheet, so then just move it / copy it to wherever you need it...

Other "solution" could be a mapkey that opens "iso22081_note.drw" and then user can copy+paste the draft group into your new drawing...

I know it's not quite what you were asking but with some training, I think it would help your users add standardized notes to your drawings.

[Mat]

Thanks @pausob for mentioning mapkeys.

I will try generating the draft group via a mapkey.
If that works, maybe i can implement an according web.Link function in our supporting App

( We use here a javascript based internal webpage to simplify certain creo functions, e.g. setting parameters, setting drawing frames, exporting data in a bunch of format at once with filenames based on model's parameters, etc)

[StephenW]

Maybe I misunderstood.

Does it always look like the image, but only with different values? If so, a symbol with variable text would be perfect.

My quick symbol attempt is attached (creo 6)

[Mat]

Unfortunately, the components "A B C" (reference planes) are also dynamic.

(Creo prefers references with single characters as names, that is why "Hello" and "World" is underlined)

[StephenW]

Ya, if you must have the GD&T reference frame truly connected to the model datums, then I don't know how to make that happen.

The symbol could easily be modified to include the datum names as variable text but they would not be connected to the datum names in the model. Your users would have to modify them to match. It's a step in making it quicker but not without manual intervention.

[Mat · Accepted solution]

I think, I have got it (works so far for me).

By using the "Additional text" option of "geometric tolerance" feature, I no longer need a draft group.

Everything fits now in on single mapkey:

mapkey iso22081 @MAPKEY_LABELiso22081;~ Command `ProCmdDwgCrGtolSpecTol` ;\
mapkey(continued) @PAUSE_FOR_SCREEN_PICK;\
mapkey(continued) ~ Command `ProCmdPmaOptGtolType`  `Profile of a surface`;\
mapkey(continued) ~ Command `ProCmdPmaInputGtolValue`  `0.2`;\
mapkey(continued) ~ Command `ProCmdPmaChkSldPnlGtolTxt`  1;\
mapkey(continued) ~ Trail `main_dlg_cur` `Geometric_Tolerance:ProCmdPmaChkSldPnlGtolTxt` \
mapkey(continued) `RibbonPanelsOnActivate_ProCmdPmaChkSldPnlGtolTxt` ``;\
mapkey(continued) ~ Input `ProCmdPmaChkSldPnlGtolTxt__panel` `PH.abv_txt_area` `Tolerances acc. to ISO 22081`;\
mapkey(continued) ~ Command `ProCmdPmaChkGtolAlgnAbvTxt`  `Align_Left`;\
mapkey(continued) ~ Input `ProCmdPmaChkSldPnlGtolTxt__panel` `PH.bel_txt_area` `linear size: ±\
mapkey(continued) 0,3\nangular size: ±0,5° \nTEDs acc. to 3D-model`;\
mapkey(continued) ~ Command `ProCmdPmaChkGtolAlgnBelTxt`  `Align_Left`;
mapkey(continued) ~ Command `ProCmdPmaChkSldPnlGtolTxt`  0;\
mapkey(continued) ~ Trail `main_dlg_cur` `Geometric_Tolerance:ProCmdPmaChkSldPnlGtolTxt` \
mapkey(continued) `RibbonPanelsOnActivate_ProCmdPmaChkSldPnlGtolTxt` ``;

[StephenW]

That's a good solution.