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Drag angles in Pro E

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PeterS369

Mechanical
Apr 4, 2014
4
I have connected a part to an assembly with a pin constraint and can drag it around the axis.
I need to know what the angle is that I am dragging it to, preferably while I am still dragging it.
If I use ROTATION AXIS in the PIN constraint, I can see the angle but I lose the drag and if I select the drag then I lose the angle display.
Also I can't switch the dimensions to get this angle display's internal name to use in a RELATION.
Is it possible to do this in any version of PRO E.
Thanks in advance for any information.
Peter.
 
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Peter,

Depending on the version of Creo/Proe you are running you can setup an analysis either saved or a Feature. The saved analysis would be the way to go. You can create a live updating annotation which can be shown or hidden from the Saved Analysis dialog. There are options to hide all saved analyses, or through the dislog you can add custom names, redefine and toggle visibility of the analysis by cliking on the eye symbol. The less costly versions of pro can do saved analyses but cannot make a Feature that gets updated with Parameters that can drive relations. You may also be able to create a Annotation Datum Feature, but the Saved Analysis is a better suggestion.

What version of PTC Parametric product are you using, I'd assume WF5 because that was the only one that was stable without as much Menu Manager BS.


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Hi Mike,
thanks for the information that does more or less what I asked for.
However, the saved analysis displays the angle but does not live update unless I stop the rotate and regen.
This is probably because I am using WF3. Also it doesn't show the internal name, so I can't access it for relations.

The annotation datum feature does display the angle and updates in real time when I rotate the part. I can also get the internal name (ad4:1), but when trying to use it in relations it says "cannot assign to a part driven function".

Being able to use this angle in RELATIONS is very important, otherwise I have to do several steps and regens where it should be automatic.
What I wanted was to rotate a part and when it reached a predetermined angle, it would (through RELATIONS) change a dimension on another part.
I thought that this would be a fairly simple action for Pro E.
Without being able to have RELATIONS recognize this angle, changes everything.
I noticed a function for relations called EANG but I can't find any info in help or on Google. Have you ever used this?
Thanks again for your input.
Peter
 
The internal name for a saved analysis result is the name of the measurement + name of the analysis feature.

There's an "_FID:" part to the overall name as well, so you may find it in help or on the web. I'd say using it in relations is the only reason the analysis feature exists.

I'm away from the needed reference material.
 
Hi Guys,
thanks for your suggestions which does just what you say. But unless I am misunderstanding it, I still end up with a static angle that requires a few moves to complete.
I have to stop the rotation at the right angle and regen, then click the UNDO in the relation window to reset the relations to current values and run again. It is easier to change the dimension on the other part manually.

What I was hoping for was that while I was rotating (dragging) an assembly around a center, the program would dynamically recognize the angle.When it reached a pre determined angle an "if" function would automatically change the dimension on another part.
Easy --right?

With a PIN or CYLINDER constraint, in ROTATION AXES, It displays the CURRENT POSITION angle around the object which changes dynamically when I move it but I can't access the angle name to use in a relation. Go figure!

Using an ANNOTATION dimension is the closest to what I want and this shows the name (ad4:1) but it can't be used in relations (cannot be assigned to a part-driven dimension).

I find it hard to accept that such a seemingly simple task is so difficult if not impossible to do in Pro E.

I have concluded that the action that I need is probably not available on WF3 or at least is way above my level. So I have decided to try some other method.
I sincerely thank the people who helped me with my questions. I learned a lot, even more than I wanted to.
Thanks Peter
 
With no picture to guide help, all I can offer is to create a mapkey (possibly a single character) that increments the angle you want and relations to drive the behavior you want. Instead of dragging with the mouse and not getting the result you want, you tap on the key and do get the result you want.

You can create the measurement feature in the part in the context of the assembly and use the value there to drive the part.

It would be nice if Pro/E worked the way you described, but it is a procedural modeler with some interactive features attached. The procedure is the list of actions to be taken, from start to finish, including relations, in order to generate the finished model. There presently isn't an ability to re-evaluate all the geometry on a continuously variable basis.
 
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