Changing number of digits in thread call-outs 1

Since the thread notes are feature-based parameters, you can edit the way they appear both in the drawing and models.

First create the thread as required. The note for thread size ( say 28 unc, is shown as 28.000 unc). In the drawing mode, select to display NOTES in the SHOW/ERASE window, and pick the cosmetic thread.

When you see the thread size (28.000), select DECIMAL PLACES, and enter "0", and pick the thread size value. It now becomes "28". If you do a SWITCH DIM, you will see it written as (or something like below);

THREAD_SIZE:FID_XXXX [.0]

The [.0] indicates that there are no sig. figs.

Unfortunately, there is no automatic method to change them all to read 0 sig-figs, so it remains a one-at-a-time process. This procedure will keep the value at "28" even after regens!!


Steve

Thanks Steve,
Yup, I tried that - to no avail.
Here is my problem;
I get something that looks like this:10-24UNC TAP DEPTH 10.000
If I go into the model normally I can change the NUM_DIGITS option under the DIMENSION menu to change individual holes - no problem.
The problem comes when I create a hole using a custom .hol file which I have modified from the original. We use all of the standard Pro/E hole parameters - we have just modified the .hol files to show a little less info - particularly on UNC/UNF and on Metric clearence holes. For some reason with the custom .hol files,I cannot change any of the depth sig. figs.
I am willing to accept the fact that I may not understand fully how to create a custom .hol file - but if it is another bug on the PTC end - completely unacceptable!

Thanks for your help,

cheers,

JW

I see, I was thinking your were using Cosmetic Thread, rather thatn the Hole Feaure. Scrath my last post (which is valid for Cosmetic threads only).

I will look into this on Monday.

Steve

Hi Steve,
After posting my question last week, I tried messing with any and all commands or config. settings to try to get some results. I decided to try the usual techniques one more time. I went into the model clicked on DIM_COSMETICS, NUM_DIGITS - I then typed in 0 instead of 3 in the command bar across the top of the screen, then selected the thread depth and hit DONE, REGEN and amazingly, the thread notes in my drawing updated to a depth of 10 instead of 10.000! After a moment of disbelief, I set the dec. places back to 3 just so I could try it again. I then spent an hour trying to change them back to 0,1 or 2 places - no go. I tried every possible combination of commands in an effort to duplicate my success.
I would appreciate it if you could verify for me that I did not imagine this......

cheers,

JW

JW,

Will look at it on Tuesday. I will try it out in Wildfire too.

Steve

I tried this and it worked for me

You need to get the note to display in the PART model. Clicking the hole itself will not help. When the NOTE is displayed in the PART, it can be selected, and right click to MODIFY. This will pull up a window that you can use to edit. I have changed it back and forth with a few numbers and it always updates the drawing and saves the changes. I can put in any value, even if it is unreasonable. All this is from the standard hole menu, no customizing.

Stressriser,
Thanks for your input.
I tried that approach also. As soon as I regenerate the model, I am back to a thread depth of 10.000
Problem is - we use the batch utility to print off all of our drawings. The batch utility opens Pro/E and unfortunately regenerates before printing - resetting all of the model notes....

thx

JW

I have one "Last ditch" effort of advice:
I can put anything in the thread call-out, I even put in the word "Bozo" and regenerated, save, called it back and printed it.

Every computer is different. My computer does not update drawings when I change the part. No one knows why...... I always get the wierd computer. I have to edit the display mode to update parts, no one else has that problem. Try editing the thread call-out on someone else's computer, and then try another...you never know, this is all I can think of at this point, other than editing the batch file you use to print, and take out the regen.

SR

Looks like I got it - finally!!
The trick seems to be selecting the number of digits in the model and then hitting redefine.

Here is the sequence:
MODIFY, DIM_COSMETICS, NUM_DIGITS then type in the number of digits in the command bar. Next, select the feature or dimension and hit done. The change will not take effect until you select FEATURE, REDEFINE. Select the hole and select the green "check mark" in the hole feature dialog box - and your done.
I don't know whether or not it is supposed to be this cryptic-but it works for the build of 2001 that we are using.

Thanks to Steve and SR for all of your help......

cheers,

JW

Ah Ha! I never noticed that...seems pretty easy huh? Congrats and thanks fer teaching us something new.

Well, this is what I did today.

I made a part with a hole feature and threads. The thread depth was given as 1.000. In a drawing calling the part, the dims were shown for the hole feature, and the complete string "1/4-20unc-2b-1.000...." was shown.

I selected FORMAT/DECIMAL PLACES and set it to "0". Pick the "1.000" text and MMB click. Update Views and now 1.000 shows as "1". In the 3d part, it also shows as "1", even after REGENs.

I went back to the drawing, saved it and closed it. Erased Not Displayed and opened it again. Still showed "1". Changed the Decimal Places to 2 units, now shows "1.00". The same appears in the 3d model.

So for hole features, changing the Decimal Places works fine.

Steve

Hi Steve,
Thanks for looking into that for me.
I just tried that again - no go. I get the message, "cannot modify number of digits on selected item".

Could just be the build that we are using.....
If how you describe it, is the way it is supposed to work, it seems like a quick and easy way to adjust tolerances.
For now though, I don't care how I have to do it - as long as I can change the note and still be able to regen.

cheers,

JW

Bye the way......
Do you happen to know the syntax for calling up counterbore and countersink info into parametric notes?
I saw it posted once before - something like: &cbore_dia, and &cbore_angle.....can't quite get it.