Pro/ENGINEER Tips & Tricks: Drafting

Drafting

• Creating Drawing sheet overlays (20060203)
  
• Using Extended ASCII characters
• Creating Geometric Tolerances using text
• Creating a format with automatically updating model parameters
• Using the @ character in Notes and Dimensions
• Creating DXF Files

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Using Extended ASCII characters

I don't know the sequence for all Operating Systems to directly type in an ASCII character in a note, but for now the following workaround is available:

First of all make sure you have configured Pro/E to use a graphical text editor for editting notes. SGI users should add the following line to the config.pro file:

PRO_EDITOR_COMMAND jot -f

E.G.: If you want to use the micro-sign type in <ALT>-181 (Hold down the <ALT>-key while typing 181) and complete it with the &ltESCAPE>-key. You will now see a µ.

Quit the editor to return to Pro/E and you will see the extended character added to the note.

You can use the script pro_ascii to create an ASCII table from which you can copy characters to your Pro/E note by marking it with your left-mouse-button and dropping it in the note with the middel-mouse-button.

Here is a list of available Extended ASCII characters:

161 = ¡ 186 = º 211 = Ó 236 = ì
162 = ¢ 187 = » 212 = Ô 237 = í
163 = £ 188 = ¼ 213 = Õ 238 = î
164 = ¤ 189 = ½ 214 = Ö 239 = ï
165 = ¥ 190 = ¾ 215 = × 240 = ð
166 = ¦ 191 = ¿ 216 = Ø 241 = ñ
167 = § 192 = À 217 = Ù 242 = ò
168 = ¨ 193 = Á 218 = Ú 243 = ó
169 = © 194 = Â 219 = Û 244 = ô
170 = ª 195 = Ã 220 = Ü 245 = õ
171 = « 196 = Ä 221 = Ý 246 = ö
172 = ¬ 197 = Å 222 = Þ 247 = ÷
173 = ­ 198 = Æ 223 = ß 248 = ø
174 = ® 199 = Ç 224 = à 249 = ù
175 = ¯ 200 = È 225 = á 250 = ú
176 = ° 201 = É 226 = â 251 = û
177 = ± 202 = Ê 227 = ã 252 = ü
178 = ² 203 = Ë 228 = ä 253 = ý
179 = ³ 204 = Ì 229 = å 254 = þ
180 = ´ 205 = Í 230 = æ 255 = ÿ
181 = µ 206 = Î 231 = ç
182 = ¶ 207 = Ï 232 = è
183 = · 208 = Ð 233 = é
184 = ¸ 209 = Ñ 234 = ê
185 = ¹ 210 = Ò 235 = ë

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Creating Geometric Tolerances using text

When you are trying to create a specific Geometric Tolerance but are unable to make it look like the way you want, here is a non-parametric workaround by creating the tolerance using only an attached note.

 

 
 
 
 
 
 
 

 Create a Note with a leader and construct your Geometric Tolerance with the box option. The following text

@[^Af^B@]@[0,3@]@[B@]

will look like
 
 

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Creating a format with automatically updating model parameters

Create start parts which already have your standard parameters defined such as: DESCRIPTION, MATERIAL, ARTICLE_NR, etc.

 

 
 
 
 
 
 
 

 When users start a new part they are automatically prompted to enter a value for most of the parameters. This can be accomplished with a mapkey that modifies the parameters (#setup; #modify; #parameter).

 In your format create a table in which you define a REPEAT REGION for each field where a parameter needs to be automatically updated (#table; #repeat region; #add; #simple). Note that you will have to merge fields to create a field with a correct size (#table; #modify table; #merge).

 In each repeat region put the following text (#table; #enter text):
 
 

        $mdl.param.value

Now create a filter (#table; #repeat region; #filters; [click region]; #add) for each repeat region like this:
 
 

        $mdl.param.name == DESCRIPTION

In this example you have told Pro/E to only display the value of the MODEL parameter DESCRIPTION in this particular repeat region.

 With such a table all parameters will automatically be updated if you add a model to an existing drawing.

It does not matter if you put the format on the drawing first and then add the model to the drawing. You will only have to do a #regenerate; #draft; to show the parameters of the model on your drawing.

 You will need Pro/DETAIL and Pro/REPORT to be able to do this.

 Download an example format table here: UNIX Compress (11k) or Zip compressed (6k)
(You could also use uncompre.exe to uncompress a UNIX compressed file under DOS)
NOTE: The format will become empty when you delete the model from your drawing and add a new one. It will not update anymore. Workaround is to replace the format or to change the model attached to each repeat region in the format table with the command

#Table; #Repeat Region; #Model / Rep

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Using the @ character in Notes and Dimensions

When creating a note or modifying dimension text you can use the @ character for several purposes:

BEGIN	TEXT	END
@[	Enclose text in a box	@]
@+	Superscript text	@#
@-	Subscript text	@#
@o	Attach placeholder of multiple line leader note to this line
@D	Dimension displayed as a numeric value
@S	Dimension displayed as a symbolic value
@O	Don't Display Dimension

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Creating DXF Files

I did some research on the DXF file creation by Pro/E and here are my findings.

Note there is a bug concerned with exporting a DXF file to large directory paths. Apparantly old builds of Pro/E R2001 crashes when the entire pathname exceeds 64 characters. This is solved in build 2003010.
See also TAN 110924

Since R2000i2 (build 2001000) Pro/E creates v13 dxf files. Pro/E R2001 creates v14 dxf files.

One thing about these version dxf files is that they can't be imported into Word. See: http://www.ptc.com/cs/tpi/107007.htm

Since Pro/E R2000i2 there is an option to set the dxf file format to v12, v13 or v14: DXF_EXPORT_FORMAT.  See also: http://www.ptc.com/cs/tpi/106321.htm

But the R2000i DXF files are different from the ones you can create in R2001 with the DXF_EXPORT_FORMAT option set to either 12, 13 or 14.

However, there is another undocumented option since R2000i2 which allows you to create dxf files which are more or less  the same as the ones created in R2000i. Set the option  DXF_EXPORT_EXTRACT to NO  to do so.

The creation of these old dxf files is twice (!) as fast and yields much smaller dxf files.  This option disables the options DXF_EXPORT_FORMAT and  DXF_OUT_COMMENT (an R2001 option for removing the first 4 comment lines created by Pro/E).

No documentation can be found on the DXF_EXPORT_EXTRACT option (not even in the PTC Knowledge Base: Search the KnowledgeBase ).

Note: when you use this option and create DWG files it will crash Pro/E R2001 (builds 2002140 and 2002180)!
The DWG->DXF converter by PTC probably needs the new format. So be carefull using this option.

Note2: november 2002, Just noticed that DXF export also crashes as soon as you try to export a drawing with dimensions on it.
To be continued ....

I did some benchmarks on a large assembly drawing. These are the results:
 

Version	Saving to ...	dxf_export_extract	dxf_export_format	Creation Time	File Size
R2000i	Local	-	-	1:21	7.1Mb
	Network	-	-	2:30	7.1Mb
R2001	Local	No	-	1:51	5.6Mb
	Network	No	-	2:50	5.6Mb
R2001	Local	Yes	14	2:04	14.0Mb
	Network	Yes	14	39:19	14.0Mb
R2001	Local	Yes	13	2:11	14.0Mb
	Network	Yes	13	44:53	14.0Mb
R2001	Local	Yes	12	1:58	8.6Mb
	Network	Yes	12	26:17	8.6Mb

Here a graphical display. Where the  x-axis is the creation time in seconds (lower is better).
Note that the R2001 Network 12, 13 and 14 scores are cut off (with the actual length being 2359, 2639 resp. 1577 seconds)

Why does it take Pro/E longer to create these new DXF files, you might wonder?

I'll tell you:
When exporting a dxf-file, Pro/E first creates a standard temp. dxf file called autocad1.dxf.

Now if you have set DXF_EXPORT_EXTRACT to YES (the default) Pro/E reads the autocad1.dxf file again and starts converting  it to whatever DXF file or DWG file you want.  This conversion process slows down the creation process, and it is extremely slow on networked drives. The difference between a v14 dxf file and the autocad1.dxf file is minimal. There is only a header added.

When you set the option DXF_EXPORT_EXTRACT to NO it creates a different kind of standard dxf file (old v12) also called  autocad1.dxf and afterwards copies it to the final filename.  This process is much faster since the dxf file does  not need to be converted afterwards.

Until I find a good reason to start using the newer version DXF files I'll use the old ones by setting the option  DXF_EXPORT_EXTRACT to NO. Then I'm closest to the processing time of R2000i