Changing Units of Part After part has been Finished.

[superart]

Hi,

I made up a small part in solidworks. the default unit in place was meters. However, I made up the part using centimeter values. So my part is 100 time larger than it should be.

Is there any way to easily convert this part from m to cm?

I cant do the standard "Tools->Options->Document Properties->Units" thing because although it would convert the units, the size of the part will still be the same. It will make the part 3200cm instead of 32m. However I need to make it 32cm instead of 32m.

I really dont want to start over on this part, as it is pretty indepth and I already spent a lot of time on it. I really hope someone can help me find a fast and simple way to do this.


Thanks in advance for any help.

 

[smcadman]

Have you tried Insert > Features > Scale?

Flores

 

[handleman]

You can try the Model Rescaler macro at

http://www.lennyworks.com/solidworks/default.asp?ID=20.

No guarantees, of course!

-handleman, CSWP (The new, easy test)

 

[CorBlimeyLimey]

The ModelRescaler macro is the better way to go (IMO). It does not create a feature in the tree. It simply re-scales the model as if it had been modelled from scratch.

The Scale function creates an extra feature which makes life awkward when editing the model later. The Scale function is better suited to create a shrinkage configuration for a moulded part.

 

[superart]

The ModelRescaler macro seems like a good idea. I especially like how the description says: "This is useful if you just built a model and discovered that it is larger
or smaller than intended because you forgot to change the model units
first."

However I think I'm doing something wrong. When I run the macro, the window pops up. I check off that I want to scale it down and I type in 100 for the scale factor. When I hit apply, the part disappears and almost all the the elements in the design tree turn red.

I've never used a macro before, what am I doing wrong? Could there be something wrong with the way I made the part in the first place? Nothing is red in the tree until I run the macro

 

[CorBlimeyLimey]

Are all the sketches fully defined? Undefined geometry could behave erratically when surrounding geometry dimensions are scaled.

Holes created with the Hole Wizard can cause problems when scaled.

 

[superart]

as far as I know, they are all defined. How would I know if they weren't? And I do not have any holes using the holes wizard.

 

[CorBlimeyLimey]

The undefined sketch elements would be blue.

Can you post the part for review and testing?

 

[CorBlimeyLimey]

Are the errors resolved when rescaling up x100?

 

[superart]

Yes, there are 2 blue undefined lines in the sketch that makes up the main portion of the part. I'm not sure how to fix it though. I have it dimensioned with Smart-Dimension, but it is still blue. Ill post it up if anyone would be kind enough to look at it for me.


If I try rescaling up 100x it just crashes solidworks.

 

[CorBlimeyLimey]

The longer blue line in Sketch1 should be constrained Collinear to the line shown in image #1.

The blue line Sketch2 can be constrained Coincident with the origin or add a dimension to one of the vertical lines.

Sketch3 was completely unconstrained. Just add dimensions to suit.

After applying Scale Factor of 100 Down, the modelscaled correctly but the circular pattern needed to be edited. The quantity had changed to 1 instead of 5.

 

[superart]

yes, that did it.
Thank you
:-D.

 

[drawoh]

superart,

Just a hint for the future...

When I type dimensions in on my models, I usually type the units with the dimensions, i.e. 22.5mm, 1.5in. This prevents a lot of weirdness.

JHG

JHG