dimension display

[ronfya]

I would like to change the default display of the dimensions I have in my drawings.

1. I would like them to be in Arial font but in the drawing option "default_font" I cannot select anything. I also tried to set it directly in my .dtl file for my drawing options but I only have a warning in the drawing options window saying :"warning: font not found"

2. Same for the notes

3. When I display a dimension by "&d..." in a note, it displays the tolerances in limits mode so I have 5.1 and 4.9 instead of 5

 

[vlad1979]

1. as far as I know you can only set those fonts that apear in the dimension properties window, there you can see the fonts installed, don't know how you can install others:


View attachment 3354


So see what fonts you have in that list and then enter that in default font .dtl


2. Default_font works for notes too, so if you resolve the above notes will display the same.


3. in config pro there is a option "tol_mode" set that to nominal instead of limits.


4. in drawing dtl set witness_line_offset to a value you like


5. if you want it like this :


View attachment 3355


then create a dimension and right click on the witness line to the left and in the menu that will apear choose erase and will look like above, then you can drag the dimension and arrows to whatever position.


if you want it like below :


View attachment 3356


then go to insert / break and make 2 clicks apart from each other on the witness line, then the line between the clicks will be erased.


6. in drawing dtl there is a option called view_scalled_denominator set it to 8 and also there is a option called view_scale_format set it to ratio colon


then in drawing in the lower left corner of the windowthere is a scale text double click on that and enter 1/4.

 

[ronfya]

Hoo big thanks for these ...
For the fonts it didn't work because I wrote arial_narrow instead of arial narrow. I removed the _ and it's ok.


I still have the problem of the tolerance mode though. This parameter was set to nominal but not from the beginning. It's like the drawing has some memory.

So I would like to change the property in the dimsnsion itself but it's not displayed and it's in a simple assembly drawing with lots of dimensions. I don't want to replace all dimensions so I would like to know if it's possible to display only the dimension I want to change its properties.

And one last thing, how do I display the zeros behind the nominal dimensions and behind the tolerance EVEN IF IT IS 0,00 ??
When it's 0 only 0 is displayed. I would like 0,00.

So for example 43,00 with tolerances +0,00 and +0,05

Thanks

 

[dr_gallup]

Shown dimensions belong to the model and retain their tolerance mode & values from the settings at their creation. You can select unlimited number of dimensions and change the tolerance type in mass without changing the value of the dimensions in drawing mode.

You need to change the drawing .dtl setting lead_trail_zeros to get the trailing zeros.

 

[vlad1979]

Actually if your drawing is metric then you can't show a tolerance like +0.00. Which is incorrect according to ASME. Metric tolerances should be shown with a single 0.


Only inch dimensions are to be shown with full zeros and without the zero before the comma. Like +.005 / -.000


So in conclusion metric or dual dimension drawings are OK if the metric portion show only one zero.


But if the drawing is a inch one then set lead_trail_zero to std_english


I will see if I can find the ASME and post a picture with the explanation
Edited by: vlad1979

 

[vlad1979]

View attachment 3402


View attachment 3403

 

[prohammy]

Vlad,


Very nice and concise rules for tolerances.

Kev

 

[ronfya]

Actually if your drawing is metric then you can't show a tolerance like +0.00. Which is incorrect according to ASME. Metric tolerances should be shown with a single 0.


Only inch dimensions are to be shown with full zeros and without the zero before the comma. Like

 

[benensky]

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Hi all, new to this forum.

I do not mean to hijack your post but I noticed that you are trying to double positive or double negative tolerance dimensions and I have had a question about that. This question arose since my company was bought by a European company ( I am in USA) and I have notice many of their drawings are double negative and positively dimensioned. The question is: Is this recommended practice by ISO standards or is it a company standard or a legacy style.


I was taught to draw a 1" shaft with at fit of -.001"/-.003" to the size it will be made at 0.999" and tolerance it 0/-.002" or draw it at .998" and tolerance it +.001/-.001. I have noticed that the European company commonly draws a 25mm shaft with a fit of -1mm/-3mm oversized at 25mm and dimensions it -1mm/-3mm.


I have seen in VERLAG EUROPA LEHRMITTEL Mechanical and Metal Trades Handbook they supplied us, that when drawing for dimensioning based on testing thatdouble positive or negative dimensioningis done. I was not sureif the example they gave was peculiar to that style of dimensioning or common practice for other styles too.


I hope I can get this cleared up because I will soon be required to draw to ISO standards and want to know the correct way to draw.


Again, sorry to go off topic,I just saw something similar to what I waslooking to get and answer about. If you think I should start my own thread I will understand.

 

[ronfya]

To benesky.

I don't think there is a rule of any kind about double positive or negative tolerances. I just think you write a nominal dimension and then tolerance it to have the clearance you want. That's it.
Also I think it is easier to understand 25 -0,1/-0,3 than 24,8 +/-0,1 because the first dimension is an integer and finally, the part will be manufactured as you wanted either notation you choosed.

 

[dr_gallup]

There is an ISO system for limit allowances for fits of holes and shafts. The same basic number is used for both the shaft & the hole and then a letter and number designate the basic allowance and the tolerance grade. For instance shaft 25 f8 is 25 -.020/-.053. You can have this dimension on your shaft and control the drawing display through Edit/Setup/Dim Bound. If you change that dimension to middle it will regenerate with a diameter of 24.9635,
upper 24.9800, lower 24.9470, nominal 25.0000. I believe most people regenerate at nominal for the drawing so there is no shown gap. However, if you are CNC programing from the model you will want to generate your code from middle.

 

[trueyan]

thanks for all your hardship!