Geometric Tolerance Issues

[nsgoldberg]

Was on Creo 3, just upgraded to Creo 10. I'm not happy with the new GTOL features. It seems significantly more limited than it was in Creo 3. From videos online, it seems the upgrade happened in Creo 4.

Main gripes:

1. What happened to the ability to select placement (i.e. free note, leader, tangent leader, in dim, in GTOL, etc)? You can select a reference but the ability to select how you want it displayed is greatly limited.

2. I'm attempting to add a feature control frame to a hole note. It's not possible and gives a very wonky result. There's no way to correct this within the GTOL.

I found this suggestion which I can't get working, and it's a poor workaround for what was functionally possible in Creo 3 anyway.

Solved: how to place a GTOL on a hole note - PTC Community

3. Tangent GTOL leaders (i.e. flatness and parallelism). There's no option to flip the direction of the FCF. You're stuck with whatever orientation it gives you. (EDIT: This seems to work on horizontal but not vertical tangent leaders).

4. Datum flags - no option to change your references (i.e. move it from the diameter surface to the diameter callout or a FCF attached to the dia. The only way to accomplish this is to delete the datum and re-create it.

There's more but this is just what I ran into in the last 15 minutes. I assume this "improvement" was to get the GTOL to play nicely with Sigmetrix' GD&T advisor and EZ Tol Analysis... But it's crippled the already-lacking GD&T capability of Creo. I feel like Creo 10 is a significant downgrade from Creo 3 in this regard.

If anyone has any suggestions for the above, I'd appreciate it. I honestly thought the revamped GTOL would be a big benefit to upgrading Creo (as we use a lot of GD&T on our drawings), but it's pretty disappointing so far.

[Chris3 · Accepted solution]

Not sure I can address all of these, but here it goes ...

1. Your reference determines the options you mentioned. For instance if you just place the GTOL in the drawing without associating it to the model then it is a free note palcement.
2. That solution does still work. Yes it is clumsy, no there isn't any other really better solutions. The only other solution is to "relate to object"
   
3. You can click and drag the GTOL to flip which side of the leader its on. You can also hold down shift and change the length of the horizontal leader.
4. You can change the datum reference on a right click.
   

The GTOL changes which started in Creo 4 were meant to comply with MBD. The old way didn't offer sematic references and machine readability. 

[JK_10266097]

Now how would one go about creating another datum feature from this feature control frame, for example from a pattern of holes (Creo 6)?

I can do this with the "Relate to Object" method, but not with the text editor method. The feature control frame shows, but the datum feature symbol does not, and you cannot attach one to the geometric callout now applied through the text editor.

[Chris3]

For that kind of hole I would recommend using the format below:

@D
⌵&d17 X &d18

Where D is the dimension for the thru hole. You show that thru hole dimension and then add in the other dimensions in the Dimension text box. If you start with the thru hole dimension then you won't have the problem of associating the GD&T and datum feature with the dimension. It is also the correct way to do it for MBD as you can assign the sematic references.

[j_k]

This will not include the 4X which is required when creating a pattern datum feature (all four holes lock down 5 degrees of freedom), correct?

Edit:

I've played with this a bit. You have to first create the FCF callout without any reference (floating on the drawing). Then you can use Relate to Object to tie it to the feature of size callout. After that, you can create a datum off the FCF. You can not use Relate to Object if the FCF already has a datum feature hanging off of it.