Geometric Tolerance Problem

[taik]

Hi, this is my 1st post here. I'm glad to see there're many helpful topics which help me in using PRO/E.


I'm a 2001 user. I have a problem in using GT in a 2D drawing for an assembly.


For instance, I have a.asm which contains b.prt and c.prt. I would like to add a TP for a dimension of c.prt. The TP should refer to the datum "X" fromb.prt.I showdatum "X" of b.prt in the 2D drawing. What should I do next to add a TP on the dimension of c.prt

 

[whit2498]

Does TP stand for tolerance projection?

 

[especial]

I think you are going to have to create it as note and attach it to the dim. TP is true position iam guessing.

 

[whit2498]

i think that its better practice to place toleranceson the individual partdrawings. in your case part b and c should each have a seperate drawing with datums and dimensions.


Its hard to tell without seeing the drawing.

 

[taik]

In a connector, solder tails true position isimportant. We always use plastic datum to dimension a true position for solder tails. That's why I need to di this in a assembly.

 

[dr_gallup]

Pro/E always tries to force you to only reference datums in the object where you are creating the geometric tolerance. Hhere are two ways you can work around it.

1) Create a datum X in the C part, put it on a special layer and turn it off. Now you can pick datum X (of part C) to make the GTOL in part C. There are several problems with this approach, the biggest is that if you rename datum X in the B part the GTOL will not update until you rename datum X in the C part as well.

2) Create the GTOL strictly as a note. Use the @[text@] to put the boxes around the note to make it look like a GTOL. Sometimes this is the easiest thing to do but I don't like "cheating" the system this way. When I do this I change the color of the text so I know it is a fake GTOL.

 

[donha]

Create datums in your assembly and reference the created datums. You cannot mix datums from different parts in an assembly to create GTOLS. Notice when creating a geometric tolerance there is an option in the box for "Model". Pro/E does not allow you to reference parts, only the assembly when you choose the drop down box. The part datums are only for the detail print of the part.

 

[especial]

"Create datums in your assembly and reference the created datums. You cannot mix datums from different parts in an assembly to create GTOLS."


I can't get it to work with a create datum in assembly. You also mention that can't mix datums. Can you put up an example or send me file?

 

[taik]

My friend told me to choose "the drawing" from the model option. Then, in datum references, click arrow to choose the datum of b.prt. Then you can place the GT to the dimension of c.prt which you need. But the dimension should be a "creared" dimension, not a "showed" dimension (I don't know why). I tried and it didwork.


Anyway, thanks for your help.