# need another help in dimensions...

• posted

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..

• posted

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

• posted

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

• posted

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 :-)

• posted

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

• posted

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

dimensions,

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