Custom dimensions

[TED7]

Hello,
A quick google brought up no answers for this and one guy who had the same problem with no resolution. At our company we show tolerances as limits to help machinists. Most of the time it isn't an issue working out what the nominal size is in the case of something like 10.0-10.1, It doesn't help with something like a m6 fit at 10.015-10.006 which has a nominal outside it's limits. In a former Pro/E based life this was easily done by just setting the tolerances to limits which gave the nominal size, the fit and in brackets, the size limits. Is there a way to do this in Solidworks at all? Currently the best way I can find is by manually editing the dimension text, which is in no way parametric and therefore a bad idea.

Screenshot attached of what we do now (above) and what I would like to do, manually edited (below).

Designer of machine tools - user of modified screws

 

[handleman]

There's no way I know of to actually make it parametric. You could automate the manual editing with a macro, but I think that would be as good as you could get.

-handleman, CSWP (The new, easy test)

 

[ctopher]

One option:
Select the dimension, in the middle of the parameters on the left of the screen is a section called "Primary Value". Select "Override value:".
Type in the dimension required. The dimension will stay parametric.

Chris, CSWA
SolidWorks 13
ctopher's home
SolidWorks Legion

 

[felix7502]

You could use favorites to achieve this. <MOD-DIAM>10m6 (<MOD-DIAM><DIM>) saveas favorite 10m6, etc.. After setting your dim to limits, highlight dim and click favorites. Not completely automatic, but dim remains parametric.

Sylvia

 

[mncad]

I'm not sure how much of this you do because this isn't a great solution. You could dimension the item twice. Dimension it with your fit, then dimension again with limit. Hide the left dimension line of the fit tolerance, hide the right dimension line for the limit tolerance, then align the 2 dimensions. Stays parametric, but a bit of a pain to create.

 

[mncad]

Picture of the finish dimension(s) put together to look like 1.