Creo 2 - Model Dims with Gtols vs Annotation layer display

[davehaigh]

In the past, WF4, I had a datums layer and an annotations layer. Whenever I "set" a datum feature, hiding the datums layer would hide the display of the set datum. Hiding the annotations layer would hide the display of annotations like surface finish. Dimension that had geometric tolerances assigned to them displayed like any other dimension.

Bringing up the same part in Creo 2.0, (Creo 1.0 may behave the same), has numerous un-desirable behaviors.

* Set Datums, will hide via the hiding a layer as long as no geometric modifiers have been added to it. If it has a flatness, it will not hide.

* Dimensions that have Geometric tolerances assigned to them will always display.

* If you go to the Annotations tab and erase the annotations so you have a clean model to work on. You can't get the dimensions to display when you double click on a feature to modify it.

Anyone figure out how to work models with this new weird behavior?

[cid:image001.jpg@01CD85FC.AFA52160]


David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550


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.

[bfrandsen]

Seems like toggling the Annotation Display on the View Tab, Show Group is the way to do it.
Showing 3D Annotation overrules layer settings I guess.

/Bjarne

[davehaigh]

So I don't see anything on either the view tab or the annotate tab to allow me to just turn all annotations off.

Perhaps I'm blind.

[cid:image002.png@01CD8686.D57D22E0]

[cid:image003.png@01CD8686.D57D22E0]

David Haigh

[AndyHermanson]

Its in the small dashboard. Circled in Red.

Andy Hermanson
Engineering Design Applications

tel 605.275.1040 x51114 mobile 605.310.8168
website www.daktronics.com

[TomD.inPDX]

Andrew is referring to the graphics window's dashboard. You have a show/hide annotation.

PTC did something weird with "Erase"... yes you have to "Delete" the annotation to have available for "show" again. Erase maintains the "showing" of the annotation in the detail tree of the drawings. Unfortunately, PTC has been blurring the lines between detailing in a drawing and annotating a model. It is a very inconsistent pool of muck when it comes to understanding what you want to show. It goes much deeper than that as well when you get into the Y14.41 3D annotation.

As for hiding the datum plane that has a datum tag assigned to them, I have already sent in many support requests and they continue to tell me this is expected behavior even though it is -very- inconsistent. Sometimes they will hide indefinitely as well once they are unhidden in a drawing. You will also find occasions where you get a fatal crash when manipulating the datum tag on the drawing. I already reported that one with the ability to reproduce the problem. Haven't heard back on this yet. But know that a fatal crash means lost work. File often!

We have a very long running thread on the PlanetPTC with regards to instability of Creo 2.0 drawings. It is better with M010 but overall, it still has a lot of shortcomings.

http://communities.ptc.com/thread/38943?start=0&tstart=0

Overall, when you start getting use to the quirks, you can figure a way around all these things. Knowing about them up front helps a lot.

Have you learned about Relative Accuracy yet?

[ptc-1932745]

Thanks for the insight. We are having a current problem in CREO1 where
datum tags can be defined but show as hidden in the tree and on the
drawing. We enabled a couple of config.pro options to set ASME as the
GDT std, and Y14.41 as well, but the behavior is weird. Much different
than WF5.



Is CREO2 much different from CREO1? We are using WF5, but are testing
CREO1 with much frustration, and are looking to CREO2 being more
consistent.





Christopher F. Gosnell



FPD Company

124 Hidden Valley Road

McMurray, PA 15317

[TomD.inPDX]

Indeed, Creo 2.0 M010 is quite a bit more stable than any of the previous releases. Obviously, PTC is bug-fixing Creo 1.0 as well so keeping up with the latest version is important. I know that Creo 2.0 F001 was very painful in drawings but M010 made it much more stable. It still has bugs though, and if you want to use datum tags (ASME versions) in Y14.5 (rather than Y14.41) mode doing detail drawings, it is still very buggy in Creo 2.0 and I suspect similarly buggy in Creo 1.0 since very little attention is being paid to detailing at PTC.

My end product is the PDF drawingso how I get there makes little difference. I completely dropped the Y14.41 capabilities and literally made a very comprehensive symbol to make datum tags on the fly for the drawing with the help of forum members. Similarly, all my GTOL features are notes. The only limitation I have found to date is composite feature control frames which I rarely need. If needed, I can make those as 3D annotation by assigning datum tags and using the GTOL menu.

By contrast, I do use the dimensions from the model in the drawing. I am still working on making the thread notes compatible with my drawings as well since this has changed form past methods (2000i). Short of the GD&T, my drawings are probably 90% associative back to the model. I still have trouble formating chamfer notes the way I want. Limit dimensions typically give me the most grief when it comes to display options.

We also recently found the issue with GTOL rounding as discussed on this forum. The answer from PTC support was less that satisfying and was in fact rudely truncated when I requested further information. Turns out Creo GTOL does not have all theoptions available per the standards. Again supporting the "work-around" GTOL practices on the drawing.

Depending on your company's policies with regard to drawing associativity, you will find that your "drafting policies" will likely end up being dictated by the tool. This, in my opinion, is unacceptable as I've always been taught that the tool should never limit your requirements. In my case specifically since I serve several clients each with their own interpretation of the standards. I must be able to output exactly what they dictate since "the customer is always right".

Edit: Creo 1 and Creo 2 are pretty much the same. Some menu items have been moved around. The help files are still -WAY- out of date.