Creo 2 Show Annotations - Number of features not showing

[davehaigh]

I'm in an assy drawing. I have a part with press in inserts. I want to show the dimensions for the holes the inserts are pressed into.

All the dimensions show find, I get the bolt circle, the hole diameter, and depth, but it's not showing the number of features in the pattern.

I've tried picking on the pattern in the model tree and selecting show annotations from the RMB menu. The dialog pops up, but even when set to the Notes tab no value pops up for the number of holes.

How do you show this?

I know I can go to the part and find the p#, but I shouldn't have to

Creo 2.0-m050

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.

[davehaigh]

So I went and got the p number from the part and entered that in the note. I get this which I don't want:
[cid:image001.png@01CE56CC.E2FEA760]

I want that to say 6X no space, no HOLES.

This used to work.

&p42:0 X &d13:0 x x[1]&d14:0
&p42:0 X @[{8:&d6:0}@] ON @[{10:&d11:0}@] BC{12:@+ @#}

If I try to eliminate the space between the P# and the X I get this:
[cid:image002.png@01CE56CD.266068E0]

Anyone have a solution other than dumb text??????

David Haigh

[davehaigh]

So I got several responses saying I can eliminate the space by using the curly braces.
Either of these work:
{1:&p42:0}X
&p42:0{1:X}

That doesn't solve the problem of it saying "HOLES"

David Haigh

[davehaigh]

So this syntax works:
{0:&p42:0}X &d13:0 x x[1]&d14:0
{6:&p42:0}X @[{8:&d6:0}@] ON @[{10:&d11:0}@] BC{12:@+ @#}
DO NOT BREAK THROUGH{15:@+ @#}
&G1:0 {19:@+ @#}
[cid:image002.png@01CE56DA.EB6B9A80]


Thanks to Janet Grove I have the answer for the HOLES problem.
Go into the properties for the p42 dimension and remove the "HOLES" suffix.
[cid:image003.png@01CE56E8.0E923F70]


David Haigh