Ok so i modeled a part in SW2019 in inches but thought I was in MM. The dimensions reflect the mm sizes so when I change units, the dimensions change to the mm value and part is way too big. Is there a way to preserve the original dimension numbers in SW. I used to be able to do this in Inventor by specifying to keep dimension numbers intact. Anything like that in SW?
I know if you export to an STL you can specify mm. Maybe you can export, then re import it?
or scale it knowing that 1 inch = 25.4mm
All else fails use dual dimensions on your drawing.
I just gave this a whirl and it seems to work.... I created a Design Table that included all of the dimensions in the part model then added a configuration (called mine "mm"). Then added a conversion dimension of 0.03937 to a cell. I used that conversion cell as a multiplier for each of the dimensions in the new configuration. If you're not familiar with excel, add a "$" sign before the column and row in the formula for the conversion cell. It will look like B22 when you select it for the formula and $B$22 after you modify it. That way you can create the first cell and then just copy/paste. If there are any patterns then leave those as is.
In that case, add a global variable: Scale.
Set it to 1 first.
Then edit all dimensions to * Scale.
Save the file then change Scale to 1/25.4.
Hello,
In the Equation dialog, create a global variable and set it to 25.4.
In all of your dimensions, divide by this global variable.
Not everything may be exposed and you'll have errors until you're done and perhaps after.
Are you biased by Inventor's ability in the hope that SW can too that keeps you from recreating the part from scratch?
It may be worth the while if the part cascades into other future files.
Kevin
Hello again,
Another point for just filing this under "life sucks/lesson learned" and recreating the file from scratch is that there will be accuracy lost in the conversion.
And not knowing about the part, but depending on the methods used and how many conversions take place, the loss may matter.
For example, SW's Scale command does perform math: entering 1/25.4 becomes 0.0393700787.
But this number isn't exposed elsewhere, like in Equations, so you can't add more decimal places.
You can add more numbers in Scale, but the displayed value gets rounded to this number of places. But is the displayed value used or is the number I actually typed used? Dunno.
Recreate it (and then present self won't have to punch future self over a POS file).
Kevin
Kevin Chandler wrote:
Recreate it (and then present self won't have to punch future self over a POS file).
Kevin
I hate it when that happens!
This is good advice to start the day!
Sometimes a person doesn't have the luxury of time at a given point in a project to recreate a file so I don't unless the tree is a hideous mess. Perhaps the accuracy of the calculations using a greater number of decimal places in excel is another benefit of using the Design Table. Calculating 1/25.4 can be taken out to 0.03937007874015750000000.... for as many decimal places as you select. The file will be as robust as the original. If a concern is how this file will look as a legacy file once the project has finished or much later when another designer is looking at the file, just delete the configuration that was in inches and the Design Table then save the part. If the configuration needs to be "Default" then rename the configurations in the Design Table before deleting everything.
I did this to an existing file and it took a matter minutes without rebuild errors.
Thanks to all who responded to my question. In the end, it was simpler to just edit the sketch and change the dimensions to reflect the mm value. It didn't take but 5 minutes. Thanks All!
Nope. You can try the Model Rescaler macro by Leonard Kikstra here:
Lenny's SolidWorks Resources