Showing results for 
Search instead for 
Did you mean: 
Showing results for 
Search instead for 
Did you mean: 

Attach datum to added dim in an assembly drawing


Attach datum to added dim in an assembly drawing

Looking to tap the knowledge base here...

Currently at CP2, M180

I have an associate that has created an assembly with a drawing.

In this drawing, an added dimension is created on a diameter feature from one of the components.  A datum axis is also generated and shown.

The desire is to attach the datum to the dimension.


The catch:

While this functionality is not being allowed in CP2, as I believe it should not. (but who am I to judge?)

It has been stated it can be done in WF4 (I have not reproduced this scenerio yet, but you bet I'm gonna try)

The is the same

The .dtl is the same.


Assuming this is true (yeah, I know all about ASS-U-ME) anyone have some insight?



This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

Hi Ron,

I just tried in Wildfire 4.0 but was not able to get it to work.  Maybe some additional information would be helpful.  Otherwise, let us know what you find after your testing.


Thanks Amit

I will give an update tomorrow - I think there has been some progress with getting pro to do what they want.  I'm heading out the door for the day.

So here is what we discovered / learned:

This is capable in WF4 and CP2, description below is CP2

In an assembly drawing, you can choose to show component items like dimensions, gtol, and axes.

So long as any of these come from the same component, you can "mix and match" ie attach gtol to dim or datum to gtol.

we have also found we can show or add a dim from a part, create an assembly axis then free place a gtol, using the assembly axis created in the assembly and attach the datum to the gtol, in essence faking the true association.


The dim can reside in the assembly or part, the gtol resides in the assembly and the axes resides in the assembly.  the dim is just "there" looking pretty.  The gtol is freely placed so no association resides between the dim and the gtol.  since the axis resides in the assembly, the gtol can use the datum as a reference and the datum can be placed on the gtol.  but neither the gtol or the axis can be placed IN the dimension, just physically NEAR because they reside on different components and no relation exists between the two.

FYI - for future reference

to be able to show component dimensions, I have seen two methods, I suggest this one:

select the Annotate tab

in the view you wish to work with, continuous RMB will cycle thru the components until the one desired is highlighted. LMB to select the component.

Select show model annotations icon.

the other is: select view, RMB hold for menu > show model annotations, RMB to cycle thru parts (move pointer over different locations to hi-lite different parts) select the component when hi-lighted and it puts all the dims.

Reason for this:

An interface drawing with the customer.  Many of these features are created on the components and would not normally be shown in an assembly.

Mating features and their location need to be shown.  Sometimes values are the same as the components but to build in a margin of safety, tolerances are inflated by a percentage to allow some "error control" in the manufacture of these parts.

Hopefully this was clear as mud and will be helpful in the future

I typically create datum curves in the assembly (actually I create an interface assembly that has as it's only component the desired assembly). These curves are aligned to the assembly geometry and contain reference dimensions. Then I create the datums in the interface assembly. Then I can attach the datums to the dimensions and all of them are confined to the interface assembly, just like the drawing says.

If necessary, add relations between the tolerances in the interface gtols and the underlying assy gtols, either setting them equal or adding or subtracting additional amounts.

Doing this prevents polluting higher assemblies with datums and gtols that are only of interest to the people designing to the interface while making it easy to find and audit those same datums and gtols

Obviously all the curves and whatever else would be blanked so they don't show up as required.

Last detail - I find it much easier to create datums and dimensions in the model and show those on the drawing, but create model gtols in the drawing mode. For some reason the model guys don't have a good grip on how to create gtols; probably catering too much to the 4% or less who think model based definition has some value.

Is this one of the reasons for the option:  create_drawing_dims_only

It can be done in Creo completely in drawing mode. You'll need to set the config option Stephen mentions, a couple of dtl options, and then create the gtol and add it in a specific way in order to get to show correctly. Without create_drawing_dims_only set added dims are created as model dims and you can't add the draft gtol to the added dim because it's not a draft dimension.