Unable to access set datum tag in creo 4

[bobjohnson35]

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

[StephenW]

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.

[TomD.inPDX]

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.

[bobjohnson35]

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]

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?

[Bogdan]

No anymore in Creo 4. 

Need to use Annotations.

[Wouter]

After reading about the changes to set datum planes in Creo 4.0 I do understand the reasons behind the changes and think it actually might be a good change looking at the future of MBD (Model Based Definition) and compliance with ISO/ASME standards.
However, there is a major flaw in the new system in that you can only use geometry to create a set datum plane. This is nice in theory but it does not match our beloved real world situations.
In the parts I design a often have datum planes that are -NOT- actual surfaces of the part. Now I cannot create a set datum plane from a standard datum plane. Some (simplified) examples: When I have a datum plane defined through 2 axes of 2 cylinders; or a datum plane through 2 points and perpendicular to another datum plane the actual datum plane does not exist in the geometry. The same goes for when I have a datum plane through 3 points on different surfaces. And so on...

Unfortunately this is another good idea not thought through well. I really hope they fix this soon!

[Chris3]

If you have datums defined by points you should looking into using datum targets.

As for a datum on the axes of 2 holes, you can always create a surface feature and then hang the datum feature symbol off of that. You could also just use a note or some words to explain your intent.

[Wouter]

First of all, thank you for you reply Chris! I am familiar with the concepts GD&T and have been using it in technical drawings for many years. My issue is not how to show such features in the drawings, but with how to create them in 3D mode in Creo.
When using datum targets to define a datum plane I still need that datum plane as a feature in my 3D model with the corresponding datum tag. The same goes for my other example of the datum plane through two axes.
I did think of creating a planer surface to attach the datum tag to, but in my opinion creating a planar surface in addition to the datum plane itself just to attach a datum target to is kind of silly. It also adds geometry that can be a nuisance when modelling, because such surfaces can block the view. To prevent that from happening I'd have to manually put them on layers and hide those (almost every time I change my layer status, since I often work with surfaces and hence visible surface layers or all layers visible).

I'm hoping for PTC to fix this asap or for somebody to find a better way (easy, robust and without side-effects).

[Chris3]

If you are hoping PTC is going to "fix" this you are going to be waiting a long time. As stated in the YouTube link below from PTC this is the new standard workflow. DFS can not be attached to datums.

https://youtu.be/poJLJy3CcLg?t=90

Obviously if you use the surface feature work around you can make the surface area very small such that it shouldn't interfere with your work. There are other workarounds (like making your own symbol) but they all have even worse downsides.

[Wouter]

Yes, the new workflows and enhancements.... I've seen those videos. As I wrote before I do understand understand the reasons behind the changes and don't think they are bad, but unfortunately PTC did not take into account that all possible real-life situations will never be covered by the standards. So there will always be the need to be able to do things beyond the standards (not meaning ignoring standards).

[LawrenceS]

The other problem is that now Creo will accept 3 datums with the same letter but attached to 3 different surfaces!!! 

1. One for the old datum creation method.
2. A second for the new datum method when created in the model.
3. A third for the new datum method when created in the drawing.

In addition,

• New gtols don't recognize old datums created in Creo2
• You can create with new gtols with datum letters that don't even exist and it will allow it but warns you.
• Datums cannot be displayed with dimension with Limit tolerance or text on additional lines because they overlap. ( https://www.ptc.com/en/support/article?n=CS293639 )

Result is some pretty upset Engineers and Drafters!  We have Creo4 M050 but according to their support logs these problems also exist in M060.  We shall see about M070 coming out at the end of this month.

[Wouter]

I've been creating technical drawings in Creo 4.0 M060 over the last weeks and it feels like it's taking me more time than ever before due to the huge amount of annoying bugs. E.g.:

* Datum planes disappearing from views (I must hide and unhide the layer to bring them back).

* The text editor for notes is still a complete disaster. In the drawing it's not WYSIWYG, it shows e.g. wrong space widths. The text editor itself adds formatting at places where it should not and even adds formatting back after having manually removed it. Some symbols are also missing, eg the AD symbol for altered default.

* Some options are only available wit RMB, probable forgotten in the menus?

* Dialogs still don't remember their size and position.

* Annotation features e.g. don't allow selection multiple surfaces with a leader for a GD&T tolerance of surface profile and they cannot be added after creation. Standalone annotations di allow this.

* After converting such standalone annotations into annotation features many references are added (went from 3 to 6!?) and all had a red dot indication they had failed.

* It's still not possible to put text in a rounded box (like an inspection dimension).

* And so on, and so on....

I'm really disappointed PTC keeps failing at implementing (often good) ideas in a workable, stable and user-friendly way.

[LawrenceS]

Inspection using rounded box works for me:

[Wouter]

@LawrenceS:
Rounded boxes work for inspection dimensions, but not in texts like e.g. in notes.
Rectangular boxes in texts work by using @[boxed text@]

[Chris3]

@LawrenceS Don't expect the things you mentioned to ever get fixed. PTC will say that this is the new workflow and you need to upgrade your old set datums to the new standard DFS.

I can say that in M060 they improved it so you can drag datum feature symbols off the surface in the drawing. It be worthwhile to upgrade for just that.

[LawrenceS]

How do you add the datums so that you can drag them off the surface?  I am testing M070 which just came out and I cannot do that with the ASME Y14.5m datums [-A-]

[Chris3]

@LawrenceS Dragging model created feature datum symbols off the surface only works in drawing mode. In MBD you still can't do it. I haven't tested M070 but you can drag off the surface in M060.

[dschenken]

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 · Accepted solution]

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????

[bobjohnson35]

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:

[StephenW]

@bobjohnson35, Please mark that video as the solution so the poor next guy looking may come across the post.

[TomD.inPDX]

Here is hoping that also solves the insessant crashing of Creo when manipulating datum tags in drawings.

[StephenW]

@TomD.inPDX, I haven't had any crashing issues with datum tag manipulation in a long time. I *think* they got that "enhancement" iron out. I do remember it happening but completely non-repeatable but nevertheless completely frustrating.

[TomD.inPDX]

Thanks Stephen.  There is hope then 🙂

[Bogdan]

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.

[GaryLinscheid]

Set the config.pro option default_gtol_owned_by_model to yes

[Chris3]

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.