Drawings...how many problems!!!!

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- edoardo fiorani
  
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posted
19 years ago

Tue, Feb 15, 2005 1:28 AM

As I usually do,i'm asking your help again.now I'm learning how crating drawings and i have the typical problems of the begginer.

1st) I noticed that Pro/e WF creates the dimensions automatically.But sometimes the dimesions are too much dense.Is there a particular command to prevent this mistake, caused by my so poor experience???

2nd) In Europe ,as you certainly know, we draw following the ISO standard that quite different form ANSI ones .In particular we have a different way of drawing the matching HOLE-SHAFT (e.g H8/h7) and the TREADS (e.g M12 x1.5).How could i draw them with PRO/E ???

3rd)Limit tolerances displayed as upper and lower limit. (e.g 15.00 +0.01 -0.05) Plus minus tolerances displayed as nominal with plus-minus tolerance when the the positive and negative values are indipendent

4th)+- Symmetric tolerances displayed as nominal value with a single value for both the positive and the negative tolerance

5th) how could i display the formats that give me the possibility of dimensioning a tolerance "as it is" ?

I hope to have been clear.And please be patient if my questions are quite stupid.I thank you so much for the help that you offer me. kind regards edoardo

- L
- LouR
  
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Vote on answer
posted
19 years ago

Wed, Feb 16, 2005 12:33 PM

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- David Janes
  
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posted
19 years ago

Wed, Feb 16, 2005 1:18 PM

Select/highlight the dims (they may already be selected if you already showed/created them). RMB 'Cleanup Dims'. Select offset and spacing and whether you want snap line created at the same time; hit OK.

The selection of drawing standard is done in the drawing setup and saved in a drawing setup file. This can be loaded, edited and saved with 'File>Properties>Drawing Options'. For your drawing options file to load each time you create a new drawing, go to 'Tools>Options' and point the option DRAWING_SETUP_FILE to your drawing options file. Save these settings in a place that will not be overwritten by a new installation of Pro/e.

First, in your drawing setup file, make sure TOL_DISPLAY is set to YES. Otherwise, the selection of different tolerance modes will be greyed out. To change the tolerance display, select one or more dimensions, RMB 'Properties' and select the mode from the drop down list and fill in the tolerance value if different from the default one. To set the default tolerance value differently than Pro/e's default assigns, set the options LINEAR_TOL_0.0, etc. to the values for each number of decimal places each 'template' shows.

Caution: this setup so far will display all values in drawings with either default or assigned tolerances. If you wish them to display, univerally, without tolerances and to display tolerances only by accessing 'Properties' for selected dimensions, set the option of TOL_MODE in 'Tools>Options' to NOMINAL.