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ptc-1412741-Visitor
1-Visitor
November 21, 2014
Question

mm dimensions in drawings

  • November 21, 2014
  • 10 replies
  • 5915 views
Hi All,

I know how to display mm's as the secondary dimension in a drawing.

The key is that I only want to display them on select dimensions on one sheet?

By changing the drawing options it appears to apply it to the whole drawing.

Doug Pogatetz
Northrop Grumman Corporation
Rolling Meadows, Illinois

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10 replies

W
wfalco16-Pearl
16-Pearl
November 21, 2014
Don't think you can discriminate.


On Fri, Nov 21, 2014 at 05:40 PM, Pogatetz, Doug (ES) wrote:




Hi All,



I know how to display mm's as the secondary dimension in a drawing.



The key is that I only want to display them on select dimensions on one
sheet?



By changing the drawing options it appears to apply it to the whole
drawing.





Doug Pogatetz

Northrop Grumman Corporation


Rolling Meadows, Illinois





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B
BobSchwerdlin1-Visitor
1-Visitor
November 21, 2014
ANSI standards dictate that if you have dual dimensioning on any single print in the package then it's required on all sheets - unfortunately. PTC follows ANSI standards. Sorry.

I've wanted to be abler to that for a VERY, VERY long time, but no-go-joe.

Bob Schwerdlin
Sr. Design Engineer,
Dukane Corp.
2900 Dukane Dr.
St. Charles, IL 60174 USA
630-797-4974 direct
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M
mlocascio1-Visitor
1-Visitor
November 21, 2014
Doug,



Yes, I would imagine that any dimension style would be a global decision for
the drawing. That makes sense.



Mike Locascio


P
ptc-1412741-VisitorAuthor
1-Visitor
November 22, 2014
Thanks for pointing that out. Guess that is why it can't be done in Pro-E.

While we do adhere to ANSI standards, I am working an IRAD project and with common sense, I do have a bit of creative license.

I asked around the department and someone here had done this.

In part mode, go to tools > relations, and define variables for the dimensions you want shown as dual, such that the values of the variables are the values of the dimensions in the units you want (For example, your relations could be: standard_dim1 = d4/25.4; standard_dim2 = d7/25.4; etc.)

In the drawing, right click the dimension to be shown as dual and select properties, then choose the dimension text tab. Type "[&<variable name=">]" next to the @D of the text. (For example, the text would be: @D [&standard_dim1]). This should now show the dimension in both units.

It does stay updated. As long as one doesn't have too many dimensions to convert this is an option....

~Doug
M
mlocascio1-Visitor
1-Visitor
November 22, 2014
Pro/E Guys,



I hear that you can do that kind of thing with AutoCAD. NO, I don't
recommend using AutoCAD - not at all. That would be TOTALLY wrong. As a
design tool AutoCAD...well...let me put it nicely..it SUCKS!



If you want to play by AutoCAD rules I will give you a comparison to think
about. Running Pro/E like AutoCAD is like buying a Cadillac and pimping it
out to look (and drive) like a Pinto, exploding gas tank included.



Michael P. Locascio


P
ptc-1412741-VisitorAuthor
1-Visitor
November 22, 2014
I am not quite sure how to control the number of digits on the custom secondary unit though. It is not controlled by the primary dimension.

Thanks to Bob and All for pointing out that it can't be done in Pro-E, so I could stop looking! 🙂

~Doug
B
BobSchwerdlin1-Visitor
1-Visitor
November 22, 2014
Oy-Vey. That sound painful.

Happy Friday.

Bob
D
dgschaefer21-Topaz II
21-Topaz II
November 22, 2014
Doug,

You can turn on unit sensitive relations (under the Utilities menu in the relations dialog), assign the unit mm to your new parameters and then only have to put this in your relations:

standard_d4 = d4

Proe does the conversion for you. Keep in mind, you have to select units sensitive in both the initial and post regeneration sections.

Also, to control the number of digits display in the drawing you'd put this in your note:

& standard_d4[X]

Where X is the number of digits you want displayed.

--
K
KENTJORGENSEN1-Visitor
1-Visitor
November 24, 2014

I'd opened a call with PTC and asked about being able to selectively turn on dual dimensions and was told that it wasn't possible.


This is quite straightforward in AutoCad, which I still use for schematics and 2D layouts where ProE's sketcher sucks wind. (Not to mention the easeof drawig with colors and linetypes)


We've got a captive shop, so the drawings aren't required to be ANSI. Our work is mostly in inch units, but I'd prefer to call out dual-dimensions on metric bearings and such because its an easy double-check on those oddball numbers on the print.

K
kimndave91-Visitor
1-Visitor
November 24, 2014

You're stuck at the bottom of a demand well. Not enough customers for PTC are asking for this to happen. 2D is the primary mode for Autocad so I imagine their well is much shallower and Autodesk was more interested in this sort of effort. At the same time PTC is looking to support the 3D model based engineering, so their drafting focus is weak.


If you have time this is an interesting read on Autodesk http://www.cadhistory.net/08%20Autodesk%20and%20AutoCAD.pdf and their history and PTC and theirs http://www.cadhistory.net/16%20Parametric%20Technology.pdf


It contrasts how the companies came to be and this is what drives them to be different. Having started with Computervision and recalling how inane Autocad was when it came out on 5.25in floppies, the events I recall are depicted as I remember them, so I think the writeup is reasonably accurate.

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