hello,
I have been tasked with converting all of our inventor drawings into solidworks drawings this is a problem because my company uses decimal points to determine tolerances, right now in a drawing when I have a degree that is exactly 45 or 90 or whatever it is, it wont display a point zero,or zero,zero. I have tried turning up the tolerance/precision but that doesn't do anything. I need those extra decimal places to appear if its possible.
that didn't work unfortunately.
it worked on all of my regular dims but it didn't do anything to my chamfers. I am trying to get them to display something like this.
.020 X 45.0 instead they are displayed .020 X 45
maybe here :
Document Properties / Dimensions / Chamfer / Angular Precisions...
Change none to however many decimal places you want in Document Properties > Units. I believe this should work.
May be: tried under Document properties > Units > Angle > select decimal.
you would think that would work but if your deg value is exact it automatically gets rid of your decimal places id like to find that setting and kill it! lol
So with your unit tolerance changed to have decimal places shown (in "Units" section), do you also have Document Properties > Dimensions > Zeroes > Trailing Zeros (all options) set to "Show"?
The solution Melissa Newby posted should work. I know that my drawings are set to show one decimal for angle dimensions and it shows if it's zero.
Document Properties / Units / Angle / choose the amout of decimal you want
then
Document Properties / Dimenions / Training Zeroes : Show
then
Document Properties / Dimenions / Chamfer / Angular : choose the amout of decimal you want
in DRW : Document Properties / Dimensions / Trailing Zero = Remove
but to change this setting for futur/new DRW, you have to do the change to the DOTDRW file.
(and also update the "drafting standard" file SLDSTD if you manage it).