WILDFIRE DRAWING QUESTION

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

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.

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

In a word. No.

For those of us in Wildfire, this sure seems to be time consuming.



Steve C

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.

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

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

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

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

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

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

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.

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

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]

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.

Has someone worked with the harness part of Wildfire?

I would like to see how this works.

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...