need another help in dimensions...

Hi,

I have a source drawings from which I am making models. My source
drawing is in mm but I want the model in inches and that too upto
exact(rounded) three decimal places. everytime I have to calculate the
value in the calculator or enter the formula in solidworks itself..
e.g. 123/25.4 then double click the dimensions again to truncate or
round off the value to three decimal places. It consumes a lot of time
and even chances of errors are also there... Is there any easier way
out..

Thanks in advance..
Kuntal

 

Kuntal,
"Rounding" these dimensions will eventually lead to trouble. If you have
mating features, holes-to-holes for example, when you start assembling them
the mates will likely not work. You are approaching it from the right
direction by entering the formula in the dialog box, but rounding them is
trouble. You can set the display of the dimensions (model or drawing) to
three places if you like, but keep entering the calculations.

I have seen many engineers/designers entering .188 for 3/16", or even .19
because they do not perceive the need for a tighter tolerance. But if
engineer A enters .19 and engineer B enters .188, and engineer C enters
..1875 (as it should be) - any mating between these parts will be hosed.

Richard

 

Maybe I don't understand, but I think you missed the obvious. Since
rounding to 3 places is acceptable by his statement, go ahead and create the
model as a metric part, and input all the proper exact metric dimensions,
which produces a correct model. Then, the drawing can be in inches and the
dims at 3 places.

WT

 

Set the options for your part as 'dual dimensions' with your primary
dimensions as mm and secondary dimensions as inches. This will allow you to
enter the dimensions directly into your part in mm, but allow you to see the
dims in inches also. While in mm you can still enter dims in inches by
simply adding " after the figure you put in the dimension box (eg. .75") -
you can also mix dimension types when entering them so long as you add the
appropriate dimension symblol after each (eg. 1 1/4"+12mm) - no need to use
a calculator.

When you create your drawing from the above model, set your drawing primary
dimensions to inches (3 decimal places & if you want fractions where
applicable select this option and set denominator to 64 - this will give you
a mixture of fractions and decimals) and your secondary to mm (if you want
to show dual dims in drawing set this option also). Your drawing will now
display all inserted dimensions in inches as required

Hope this helps

Merry

 

Wayne,
You're right, I went around the block to get next door. And, he can work in
a model set up for inches by simply adding a "mm" to the dims when entered.

But if I understand Kuntal correctly, he is inputting a "formula"
(100.10/25.4 for example), and getting a value of 3.94094488 let's say.
Then, double-click the dimension and remove the last 5 digits. The resulting
dim is 3.940 and eventually will cause problmes downstream with mates to
other parts. That's what I was trying to get across.

Richard

 

Agreed. Brings me back to my main point - model with the correct units &
numbers, either by setting the part units, or by something such as 25mm, and
then let the drawing handle whatever you want to manufacture to.

WT