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WILDFIRE DRAWING QUESTION

swcalvert

New member
Still being new to the whole concept of Pro/E, let me ask this question. In Wildifre, and I guess it's about the same in 2001, when I add views to my drawing and then add dimensions using the 'show/erase dialog' button, I get every dimension that was used to make the model in the view that I have picked. One- Is this the best way to get dimensions on the drawing? Two - What is the fastest way to clean up the dimensions? I don't just mean aligning them, but moving all the extension lines so that they are not ectending into the model.



Steve C
 

BobP

New member
I find the best way is to do it per feature. Click the feature you want to dimension in the model tree, then right click and choose add dimension. It's slower this way, but you do have more control.
 

swcalvert

New member
OK, I can deal with that. But, what about the extension lines running all over the place, will picking the feature solve that?



thanks,



Steve C
 

asmenut

New member
When in Show/Erase, click on the Feature/View checkbox.

This is much faster than the Model tree and easier to cleanup than the part dimension.
 

swcalvert

New member
Thanks, asmenut. At least for the one feature I tried it on, it seemed to place the extension lines outside the model. It still takes too much time, IMHO, to dimension the part.



Steve C
 

jabbadeus

New member
Go to Edit > Cleanup Dimensions. On the first tab of the dialog box, you can specify how far to place your dimensions off part geometry, and the spacing between subsequent dimensions.



Dave Martin

Torgon Industries
 

swcalvert

New member
Thanks, Dave. That does the trick for cleaning up the spacing, but it does nothing for all the extension lines that are spread out into the part. Does the position of the feature sketch dimensions have anything to do with the location on the drawing of those dimensions? I wonder if I should pay more attention to how I model and place the sketch dimensions.



Steve C
 

Moroso

New member
I think Pro/E will automatically clip dimensions when you print the drawing. I just move the witness lines out of the way with the move command
 

jabbadeus

New member
You can print to the screen to see how Pro will automatically clip extension lines. Then adjust the ones that are still screwed up.



You might even be able to create a macro and icon that will print to screen... I've never tried this, but I should. (I print to screen a lot when I work on drawings.)



Dave Martin

Torgon Industries
 

swcalvert

New member
If I'm hearing you guys right, you're saying that I don't need to manually move all the extension lines that show up on the drawing as interferring in the model?



Steve C
 

Moroso

New member
Yes you don't need to manually move the witness lines back. There is an option in your drawing dtl file called witness_line_offset that takes care of clipping the witness lines when plotting.
 

swcalvert

New member
Outstanding, you don't know how good I feel right now, knowing that I don't have to move a lot of extension lines.



Thanks,



Steve C
 

satish

New member
dear friend's



I sujest Edit>cleanup dimensions is the best method to rearrange the dimensions. but in some cases, arranging the dimensions is better.



Thanks and regards,



s.satish kumar

Design Engg.

sharjah uae.

[email protected]
 

donha

New member
I would have a bird if I called up a drawing and the extension lines were all over the place because someone knew Pro/E would clip them during plotting. It takes no time at all to clean up dimensions, take pride in your work?

This is the way I create drawings. Modeling first. Create drawing with primary views. Have the model and drawing active in session. Modify one feature at a time in the model and decide which view the dimensions need to be shown in. If no view exists, create the view in the drawing. Using Show/Dimension/By Feature and View, show all the dimensions for the feature in their respective views. If you use this method, you will ensure all dimensions necessary to create the model are shown on your drawing. I also redefine features if the features driving dimensions do not suit fit/function. This method ensures design intent is captured and most dimensions on the drawing are driving dimensions. It also ensures you have used relationships where necessary. All views are created on sheet 1 even if it is a 4 sheet drawing. Only after dimensioning is completed do I move views to their new sheets.
 

proed

Moderator
On the question of cleaning up witness lines, etc... I have to agree with donha - it takes hardly any time to clean up your witness lines.

It's just one of those things you have to do while drafting (can't expect the program to do all your work for you!!).

It would be really frustrating working on someone's drawing if they hadn't had the decency to clean things up...
 

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