rounding up....

[design-engine]

In solidworks you key in a three place decimal and set your display in the drawing to two decimal places, the geometry does not round up. Only the display will round up. In Pro/E the same scenario will force a regeneration and round up or down the geometry.

I never really thought much about it... Anyone have a preference?

 

[PRStockhausen]

My preference would be to force the change to the geometry. The nominal of a .37 inch dimension should be .370000000 not .375000000. Modeling to something other than the nominal size creates a problem for a vendor making the part from the file. He would not have the tolerance he thought he had.


A worse idea is to model a R.030 MAX as .030000000, if the vendor makes the part to the model without checking the drawing carefully and comparing it to the model, he will need to scrap about 50% of the parts. If I was that vendor, I would add money to my next bid to take the time to remodel the part.

 

[dr_gallup]

There are several things you can do if you want the geometry to be something other than the dimension nominal. Even with nominal dimensions (no displayed tolerance) you can assign tolerances. So if you want the drawing to show R.030 max. set the upper tol to zero and the lower tol to .030 then in edit/setup/dim bound set the dimension to MIDDLE and the geometry will regen to R.015. Or in your case, create a relation with the dimension set to the 3 decimal value, it will stay at that value no matter the display. Another possibility that I personally hate is use a created dimension & change the number of decimal places. Isn't that what everyone with SW does anyway?

 

[looslib]

With imperial units and a unspecified tolerance block based on decimal places, modeling to .375 and showing as .38 does change the allowed tolerance available to the shop and could scrap parts. I think you should model to what you need and show the same dimension on the drawing.


The ability for Pro/E to change the model based on the drawing dimension can be turned off.

 

[design-engine]

plus ever detail is stored in the part with Pro/E not the drawing like SW.