Drawings...how many problems!!!!

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

 

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.

 

will study PRO/E during this weekend and i hope to find the correct
solution of problems,following your advice.Another thing. How could i change
the type of line to rappresent the hiddenlines in my Drawing files.I'd like
hidden lines to be displayed by discountinous ones (Phantom or dashed).I
thank you again and sorry if I disturb you.
Edoardo