Dimension text placement

[ndk]

Hi all,


Sorry for my odd question, but anyone please tell me how to place a dimension value in proe wf 2.0 like the picture below? and can we define dimension value in fraction format, such as 1/2 or 3/8 ...?


View attachment 828


thanx all

 

[skraba]

Regarding fraction format. You can place dimension with fractional format. Just choose Properties and then on the Format field choose Fractional radio button.

 

[Blaze]

i think, you have no opportunity to place a dimension value in such a way.

 

[ndk]

that's why isometimes have tosave my pro/e drawingto DWG format for a better performance.


thanx all

 

[rgs1]

You can also set the config.pro option as follows:


create_fraction_dim&nbsp ; yes


This will set all drawings to have fractional dimensions.

 

[scubadude]

You can construct this dimension (while I've never had ocation to do it myself) by removing the dim text from the exsisting dim and adding a parametric note pointing to the dimension arrow.


Here' how... (in Pro/E 2001 that is...)


Select the dimension, right click, select PROPERTIES


Select the Dimension Text tab


Replace the @D with @O (the letter O not the number 0)


For furture reference, note the NAME of the dimension in the first box under the big note box. (in my test it was d31)


When you click OK the dimension text should disapear.


Now create a parametric note that points to the dimension by using


INSERT>NOTE>LEADER>MAKE_NOTE>FREE_POINT>NO_AR ROW


Click the location at the center of the dimension arrow, which should now give you a prompt for text. Enter the andpersand (&) and the NAME of the dimension you omitted in the previous step (ex: &d31). If the dim requires a symbol (diameter, radius, degrees, etc, you should add that as well with the symbol pallet)


When you hit enter the note should have the correct dimension value.


NOTE: since you can't attach the note to the dimension arrow, the note will stay where you placed it. If you move your drawing view, this note will not follow it.

 

[rgs1]

Scubadude,


I have wondered for a long time how to replace a dimension with text as you have outlined above, but when I replace the @D with @O (letter O) then hit OK, my dimension stays the same..... it does not disappear. Please let me know if you might have omitted any steps. I tried numerous times, but to no avail.

 

[scubadude]

Having tried this after posting it, I have the same problem. I know this is how it should work, because I've done it before. Also, it is documented in the HELP file as shown in the excerpt below. I'll check to see if there is a parameter that is set that will fix this. I tried the @S and it worked...
<H1 style="MARGIN-TOP: 7pt; FONT-SIZE: 12pt; MARGIN-BOTTOM: 2pt; MARGIN-RIGHT: 6.5pt">Text Strings</H1>
When you are editing text, dimension values appear as follows:

 

[rgs1]

Scubadude,


Thanks for any help (investigation) you can do. Many times I need to substitute a line of text instead of a dimension. This would be very helpful.

 

[dr_gallup]

You can not use the @O for part dimensions, only dimensions created in drawing mode. You can use the @S for all dimensions. So in this case, create another dimension in the drawing and change it's text to @O with a leading or trailing space (don't ask why but it won't work without some additional text). Then create your note with the &d## text. At this point the part dimension should disappear and you are left with your created blank dimension & note. You can give your note an OFFSET attachment and it will move with your created dimension & view.
Edited by: dr_gallup

 

[rgs1]

Scubadude,


YAHOOOOOOOOOO....It worked!!!!!!!


I have to print this one so I don't forget.


Thank you very much.

 

[scubadude]

Thanx dr_gallup. I had forgotten that you needed to use a created dimensionin order to blank it out. I also was unaware that you needed to put some extra text there to get it to work. I've always replaced the dim with text, so I never realized the need.


rgs1, Glad to be of help.

 

[scubadude]

PS... On version 2001 there is no "OFFSET" attachment. Must be an improvement with WF.

 

[rgs1]

dr_gallup / scubadude


Originally I only thanked scubadude (not realizing the post abt the space req'd was from dr_gallup)................thanks to you too dr_gallup........without both of your knowledge, my problem would have never been solved.

 

[ndk]

Thanks everybody.


I followed all your guides and the problem solved. But I also have small question...


when I create note with &ad### text, the dimension line disappeared and I were left with only the note. So, to solve problem, I have to do 3 steps. Please have a look and let me know is it possible to make it easier?


View attachment 852


So, I have to make a work-around. making 2 dimensions on same item. like this:


View attachment 853


and here's result


View attachment 854


you can see, the inner dimension disappeared and the note pointed to outer one. (thought the paramter is of the inner)
Edited by: ndk

 

[scubadude]

ndk,


That's pretty strange. I'm not sure why the dim would disapear like that. I managed to create one without this problem. Which version of Pro are you using? I'm only on 2001.


Another note about making the parametric note...
Since you need to 'create' a dimension in order to remove the text (using the @O) it would be best to reference the actual driving dimension in the note, i.e the dimension that you can't remove the text from. That way you can edit the value in the note to change the model. Having it use the created dim # is still better than plain text because it will at least change with the part. This gets into the philosophy of whether you prefer 'creating' dims on your drawings or 'showing' driving dims on your drawings.

 

[ndk]

I'm using WF 2.0 (M030)...


NDK