SOLIDWORKS Design & Help

Dual dimensions is the only way that makes sense, imo.

As an Engineer it is my duty to reduce the possibilty of making errors as much as possible. (Have a look at Murphy's Law :) )

Mixing dimensions is never a good solutions imo, since it leads to faults depending where the drawings are processed.

Solidworks therefore (as any other CAD system) sets the units in the templates according to the SI-unit system e.g.

Não é muito bom misturar dois padrões de medidas no mesmo desenho ou dimensão, pois na máscara do desenho já é definido que todas as medidas contidas são em MM ou IN, o máximo que costumo alertar é na legenda onde Índico o tipo de matéria prima a ser utilizado, geralmente estão em IN em sua maioria. Abraços e bons projetos.

I completely agree with TheHitman. As a company we receive drawings and sketches of various qualities and we are far more likely to quote a job higher that is received with mixed dimensions or even decline quoting it as experience has taught us drawings containing mixed methods of measurement are far more likely to be drawn and thereby made incorrectly.

With no offence intended to anyone, you have to think of machinists and mechanical engineers as idiots. The simpler the better. They are there to produce to a drawing not to spot problems or input opinion and if dimensions swap between mm, cm, inches and ft then it won't take long for an issue to occur.

You can always completely edit out the dimension wording from the edit box that appears on the left when you make or edit said dimmension. That way you can manually input the value in inches, and then also add ''inch'' next to the number to specify that said dimension is in inches, and not in mms as the rest of the drawing.

Set the drawing to in. or mm. Dimension fully. Then click each individual dimension you want to change and edit using following methods. see attached pictures. You will have to convert dimensions yourself. Multiple or divide by 25.4. I didn't convert, did this quickly.

-OMNICAD

Thank you for the input, guys.

I also agree with you that mixing the dimensions units is not the best idea.

In this particilar case the drawings are intended for presentation purposes of tubing-like products not for manufacturing and the vertical to horizontal ratio is like 3-5 meters (10-15 ft) to 50-100 mm and usually are used by people who are used to that format. So we can assume even if someone mixes the units it's not so vital.

So with the above explained do you have any ideas how to make this work :) ?

@Ares Chatzaroulas and @OMNICAD

I forgot to mention that I'm looking for an automated process (or as close as possible) similar to using the dual dimensions option which automatically adds the second set of units.

May be you can go with a note in title sheet

"All lengths in mm"

"All Diameters in Inch"?

The only way I know to do it is to dimension it all in one unit or the other. You cannot have SW automatically know. Then hold ctrl and click all of the dimensions you want to change to the other unit. On the left you will see the 3 tabs - Value, Leaders, and Other. Click Other then the Override Units check box. Change the drop down box to whatever unit you need. This keeps the dimension associated and will correctly update if you modify the model. The above mentioned method where you manually type the dimension will no longer update correctly and is asking for typos. This will even allow you to make things into fractions.

I used to make my drawings in metric but our machinists used fractional drills so I used to have to use this method all the time to change my holes to fractions.

Rob Stoll,

Great idea. I think that's the best automatization I could get. Especially that it keeps the link to the original dimension and will correctly update if modified.

Thank you!

Anytime! Its what we are all here for. Advice from a giant think tank!