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Creo 2 - Geometric Tolerances/Annotations

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Creo 2 - Geometric Tolerances/Annotations

My company made the jump from WF3 to Creo2, and I'm struggling a bit with drawings. It's been a while since I've used Pro/E, as most of my recent projects have been in Solidworks, so I may just be a bit rusty. The modeling has been easy to get back into, but I'm really struggling with drawing creation, specifically geometric tolerancing.

In the past, I would create geotol datums and tolerances in the model, and simply show them in the drawing when that time came. It seems to be a bit more complex now in Creo. After much trial and error, I've finally managed to get my geotols into the model and displayed on the drawing. It took a while to figure out, and I'm still not sure I quite grasp the new "Annotate" tab. I could create datums and geotols to my hearts content, but it was a 50/50 shot if they would even show in any drawing view. Sometimes the datum would display, but the geotol attached to it would not, or could only be shown in a specific view. I ended up deleting and recreating the reference datums and geotols several times until the eventually would display somewhere on the drawing.

One of the main things that is a bit confusing, as there seems to be no rhyme or reason as to what view you can and cannot display the annotations. The annotations I've created were placed on specific planes, but will not display on those planes/view oreintations in the drawing. If I go back to the model, and move the annotation to a different plane, the drawing does not seem to care at all. It just stays in it's current position and view. Sometime there would be several view options to display a datum target, but not the associated geotol. It's just very odd. The datums can usually be shown in multiple views, but not the associated geotol.

The other thing that has me a bit confused is hiding datums/geotols in the model. In the past, I've used the environment setting to not display notes created from taped holes, and layers to hide geotols/datums. Things seem to be a bit different. The only way I can manage to hide a geotol or datum is to right click on the annotation from the detail tree when in the annotate tab and erase it. When in the model, and in the annotate tab, the "show annotation" button will not allow me to not display the datum or geotol regardless of what I click on.

Besides that, the learning curve hasn't been to bad. It took me a little while to find the existing features and settings I'm used to using. Everything is still there, just in a differnt place. The creation of geotols/datums has alway been a bit counterintuitive, but I knew how to do it. However, with Creo I can't make any sense of it. Can anyone add some clarity, or tips, or point me to a good guide? Am I the only one struggling with detailing?

Creo2.0 M070

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Creo 2 - Geometric Tolerances/Annotations

Mike; I know your frustration and have even put in several support cases into PTC to get tot he bottom of this. All I get from them is the old "...works to specifications". PTC has been so focused on ASME Y14.41 that the drawing implementation has really suffered.

Bottom line for me, I don't use Creo's GD&T annotation. I don't even use their datum tags. I have made a custom symbol and place them at my heart's content. I make all my control frames with notes. In the very rare even then I cannot make the control frame (a double line with a single action), I will make it in the model and show the annotation.

The fact that the drawings do not open as saved is really annoying, and is actually a serious issue. This forces a designer to be extra vigilant in releasing their final version. Something there is absolutely no excuse for. But as many of have tried to get this problem before the engineers, we are simply blown off and the product does not improve. I am very much looking forward to seeing what Creo 3.0 has to offer in this regard. Reportedly, this module was completely re-written. Time will tell.

Only real tip I will give you is that you do not add a datum tag to the primary datums. Create a new datum for the datum tags by selecting a surface or axis and let that datum do that and only that. Their behavior for showing and not showing is a bit more predictable. I have found the paradox with always shown datums w/ tags in the model will flip when you show that datum in a drawing. It is one of the poorest implementations I've seen to date in Pro|E.

I am certainly not saying that my way is the best way... it is the best way for me. Many are bound by policy to make the system work and to become familiar enough with the idiosyncrasies to come up with a workable foundation. My clients simply don't need that, and they certainly are not willing to pay for the extra time it requires to manage such nonsense.

Good luck!

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10 REPLIES 10

Re: Creo 2 - Geometric Tolerances/Annotations

Mike,

Maybe Antonius will chime in, but here are some threads about using the GD&T built into Creo versus manually adding the GD&T to drawings:

http://communities.ptc.com/message/185437#185437 - built in GD&T - unstable and casues hards crashes

http://communities.ptc.com/thread/38943 - Unstable

http://communities.ptc.com/ideas/1140#comment-5496 - upgrading GD&T within Creo

http://communities.ptc.com/message/187521#187521 - GD&T and dual dimensions

http://communities.ptc.com/message/203555#203555 - GD&T issues with datums

These are just a few things.

Thanks, Dale

Re: Creo 2 - Geometric Tolerances/Annotations

Thanks Dale!

Re: Creo 2 - Geometric Tolerances/Annotations

Yesterday I managed to get all the datums and geotols on the drawing, but when I opened the drawing this morning they've all disappeared. The really odd part, is that the annotations are still contained within the model, but will not display on the drawing.

Re: Creo 2 - Geometric Tolerances/Annotations

Hi Mike,

Sorry I have to be brief but this is 99% A LAYER ISSUE.

Check your drawing layers. Also if you have any hidden sketches that control Gtols or influence them, unhide them. Turn them off by layer if you need them to dissappear in the model.

Thanks,

Brian

Re: Creo 2 - Geometric Tolerances/Annotations

All my layers are unhidden, still no change.

Re: Creo 2 - Geometric Tolerances/Annotations

I've unhidden every layer, including the default "hidden" layer. The datum tags show, but not the geotols.

Re: Creo 2 - Geometric Tolerances/Annotations

Just for the heck of it, try unhiding all of the layers in the model. Also, go to the annotations group in the drawing tree (at the top) and make sure your GTOLs are being "shown". You should see a small flashlight icon next to each GTOL being shown. Let me know what you find out.

Re: Creo 2 - Geometric Tolerances/Annotations

Hi Brian,

Ok, I think I have it now.

If the model datums are hidden, any associated geotol will not show in the drawing, period. Unhidding the datums didn't show the gtols because they were model annotated gtols, and from what I gather, they are hit or miss. Datum tags show up pretty easily, but any flatness, perpendicularity gtols attached may or may not show up. It really is a 50/50 shot. The placement plane seems to have little to no bearing on which view they can be shown in either.

From what I've experienced, it may be best to create the geotols in the drawing once the datum tags are established in the model. The datum tags can pretty much be displayed in any view, and a draft gtol can be easily added to it.

The only thing I can't figure out, is how to hide the model datums in my model without causing the associated drawing datum from being hidden. Layers are obviously not an option. I even tried the old trick of changing the drawing view layers independantly from the model layers, which no longer seems to work. The model datums can be added to a custom hidden layer and the layer can be hidden, but the datum features will still show once they used to make an annotation. Toggling "annotation display" hide the datum tag, but not the datum itself. It only toggle the datum tag display.

What's even more strange, is that the model datums are always shown in the model, but are somehow not shown in the assembly.

I've been a Pro/E user for a while, and rolled with all of the changes from 18 to Creo, but these recent changes to the drawing tools is leaving me scratching my head.

Thanks for all of your help.

Re: Creo 2 - Geometric Tolerances/Annotations

Mike; I know your frustration and have even put in several support cases into PTC to get tot he bottom of this. All I get from them is the old "...works to specifications". PTC has been so focused on ASME Y14.41 that the drawing implementation has really suffered.

Bottom line for me, I don't use Creo's GD&T annotation. I don't even use their datum tags. I have made a custom symbol and place them at my heart's content. I make all my control frames with notes. In the very rare even then I cannot make the control frame (a double line with a single action), I will make it in the model and show the annotation.

The fact that the drawings do not open as saved is really annoying, and is actually a serious issue. This forces a designer to be extra vigilant in releasing their final version. Something there is absolutely no excuse for. But as many of have tried to get this problem before the engineers, we are simply blown off and the product does not improve. I am very much looking forward to seeing what Creo 3.0 has to offer in this regard. Reportedly, this module was completely re-written. Time will tell.

Only real tip I will give you is that you do not add a datum tag to the primary datums. Create a new datum for the datum tags by selecting a surface or axis and let that datum do that and only that. Their behavior for showing and not showing is a bit more predictable. I have found the paradox with always shown datums w/ tags in the model will flip when you show that datum in a drawing. It is one of the poorest implementations I've seen to date in Pro|E.

I am certainly not saying that my way is the best way... it is the best way for me. Many are bound by policy to make the system work and to become familiar enough with the idiosyncrasies to come up with a workable foundation. My clients simply don't need that, and they certainly are not willing to pay for the extra time it requires to manage such nonsense.

Good luck!

View solution in original post

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