Thread Callouts

I am very new to ProE, but I have a lot of experience with Works and Edge. I am having trouble using the standard hole command. The problem I am having is in the note callout for the hole. I modified this .hol file so that my note if formatted correctly, but my drill is being called out as 10.500 instead of 10.5. Does anyone know of how the thread callout can be formatted so that I don't have to go in and remove all of the trailing zeros all the time. Any help would be greatly appreciated.

Again, you'll hve to edit the .hol file, fifth column of data. Eliminate any zeros you don't want to show. Hopefully, in the CALLOUT_FORMAT you didn't formatting commands like [.3] because this will force trailing zeros.

David Janes

Thanks for the information David. I will try that out on Monday.

I can see where that will work for the hole diameter where I can simply type in the text that I need to have shown, but the problem is also in the hole depth as well. If I specify that a hole is 19.5 mm deep, I would rather not have the callout saying that it is 19.500 mm deep. I am just not sure how to control this. The user can type in any depth he would like, any thoughts on how this can work?

I know I am asking the same question that many people have asked before, but it just doesn't seem to make much sense to me right now.

Thanks, Dan Brownson

Thanks for the information David. I will try that out on Monday.

I can see where that will work for the hole diameter where I can simply type in the text that I need to have shown, but the problem is also in the hole depth as well. If I specify that a hole is 19.5 mm deep, I would rather not have the callout saying that it is 19.500 mm deep. I am just not sure how to control this. The user can type in any depth he would like, any thoughts on how this can work?

I know I am asking the same question that many people have asked before, but it just doesn't seem to make much sense to me right now.

Thanks, Dan Brownson

Pro/DETAIL has its own configuration files ending in .dtl and stored initially (not customized) in the \text directory. If you customize one of these, move and rename to someplace that will not be overwritten with a program upgrade\patch operation. I think you can name it anything you want, just be sure to point to it with the config option drawing_setup_file and browse to it. To make others available when you do 'File>Properties>Drawing Options', also set the option pro_dtl_setup_dir to this directory by browsing to it.

The option that should drop the trailing zeros is called lead_trail_zeros and should be set to std_metric. The ISO standard, unlike the US Customary, bases tolerances on tolerance tables, not on decimal fraction precision. So, .5 can be toleranced the same as .50 or .500. Whether to drop the trailing zeros depends on your tolerancing scheme, whether ANSI/ASME or ISO. The ISO tolerance tables could be a whole other discussion.

David Janes

On Aug 23, 11:04=A0am, snipped-for-privacy@gmail.com wrote: add brackets and the number of decimal places you want. i.e. DRILL_SIZE[.1] will round off the value to one decimal place.

I changed the lead_trail_zeros option on the draft sheet, but I still get trailing zeros in the note. Is there something else that I am missing? It looks like the note is copied over exactly from the part file. Is there any way that I can control this in the part file.

I really appreciate your help, and I know this can be done I just don't know what I am doing wrong. I really don't want to resort to doing &DRILL_DEPTH[.0] or &DRILL_DEPTH[.1] because that would change from callout to callout.

Thanks, Dan Brownson

figured it out.

Someone had set the default decimal places to 3 places. switched it back to 0, and it works like a charm.

Thanks for your help.

Dan Brownson

I believe I may have posted too soon. when I changed the default decimal places to 0 it rounded my dimensions so now 12.6 = 13mm. Not what I was looking for either.

If anyone has any additional ideas on what I can try please let me know. I am really scratching my head on why I cant do this.

Are other users able to do this function? It seems so basic and simple, but I can't get it to work.

Thanks... again!

Dan Brownson

I believe I may have posted too soon. when I changed the default decimal places to 0 it rounded my dimensions so now 12.6 = 13mm. Not what I was looking for either.

The config.pro setting of default decimal places is a model dimensioning option. Hole note parameters are not, strictly speaking, dimensions but note parameters with values assigned from the table or the hole interface. At the same time, these should correspond to actual dimensions of the hole which you can see by selecting the hole and RMB 'Edit'. It might be worthwhile, in the drawing, in a view (not the view showing the hole note) to show the actual hole depth dimension. Assuming everything in your .DTL file is set to Metric/ISO, the Lead_trail_zeros option set to STD_METRIC. You'll notice also that there are a bunch of different values if you're using dual dimensioning. The STD_METRIC value will not give the correct results if you're doing dual dimensioning. I'm thinking that the note may display the way you want if you can get the hole dimensions in question to display correctly.

If anyone has any additional ideas on what I can try please let me know. I am really scratching my head on why I cant do this.

BTW, you may also have to change another .DTL option, LEAD_TRAIL_ZEROS_SCOPE to All.

Are other users able to do this function? It seems so basic and simple, but I can't get it to work.

Just tell yourself that it's improving every year. I figure in only another millenium of tiny incremental yearly improvements it ought to be perfected. A blink of the eye in geological terms. I'm hoping that PTC's aware of natural selection.

David Janes