I have a question. I am having trouble finding out if there is a way to scale a simple a model in Creo 4. My issue is that I would like to use my original model as the "default" of 1 and be able to scale it from there, but being able to scale it back to "1" whenever I need to. The only ways I know of are:
1.) Use "Scale model", then use a calculator to find out how to get back to your original scale of "1"
2.) Set all dims in a relation of original value multiplied by a "Scale" parameter (which would take me a long time to set up since I have 70-100 dims in my model
3.) Use "Scale model", then Save As as a separate model
We are taking a model and running several simulations on it, finding an optimum result. Our analyst would like to just take the model and use a scale factor, so he will be running several iterations, using many scale factors. Any help would be great!
Option 3 is the best.
No chance of messing up your full-scale design model.
We use that method for our SLA scale models.
Thankfully, I can easily use 2 of my 3 options without too much fuss. The analyst said he can keep moving forward with those for the time being. I appreciate your response. Thank you!
Out of curiosity, what method did you end up using?
For right now, we are just using Scale Model and using a Save As, so we can save the analysis along with the scaled models. That seems like a feasible enough direction for what we are doing now.
I really appreciate all of the responses!
You could write a relation that calculates the appropriate value to scale by so you don't have to bring out the calculator every time. It'd be nice if you could then make a mapkey that copies this value and scales the model back to 1, but unfortunately, mapkeys can't copy and paste values. 😞 You can do it with an API, though. i've been playing around with the VB API lately, and you can do all sorts of cool things to control Creo from Excel. This would be a piece of cake to do in VBA.
Barring that, though, i think the best you can hope for is a mapkey that brings up the parameter value and pauses so you can copy it yourself, then when you unpause, launches the scale model command to let you paste the value.
If you have access to the mold design extension you can add a shrink feature to the model. Using this feature you can scale the model and modify the scale factor parametrically and suppress the feature to return to 1:1 scale.
Make sure to put this feature at the end of the model as it applies to everything above it in the feature history.
Shrink by dimension—Allows you to set up one shrink coefficient for all model dimensions, and specify shrink coefficients for individual dimensions. You can choose to apply shrinkage to the design model.
Shrink by scale—Allows you to shrink the part geometry by scaling it with respect to a coordinate system. You can specify different shrinkage ratio for the X-, Y-, and Z-coordinates. If you apply shrinkage in Mold (Cast) mode, it applies only to the reference model and does not affect the design model.
Good point! You could do that with the Warp feature (transform operation), too, if you don't have the mold design module.
I have not used it recently but I think all of the warp functions are based on the use of drag handles to manipulate the geometry. This is not easy to precisely control geometry dimensionally. I would also be sure to check the geometric integrity of scale using warp, it could distort geometry such that it could affect simulation results which is the intention of the user in the original post.
If you can now scale on all 3 axes using a scale factor with a warp transform, I would be interested to understand how that is realized.
Do a warp, select the geometry and a coordinate system, choose Transform, then just click on one of the corners. Open the Options panel, you'll find a scale value. Set any scale you want, and set the Toward to "Center".
EDIT: Tried this in Creo 6. I think it's been like this for a while, but I can't be bothered to check other versions right now.
@Pettersson wrote:
Do a warp, select the geometry and a coordinate system, choose Transform, then just click on one of the corners. Open the Options panel, you'll find a scale value. Set any scale you want, and set the Toward to "Center".
EDIT: Tried this in Creo 6. I think it's been like this for a while, but I can't be bothered to check other versions right now.
NOTE: I had to move geometry corner before setting scale value in Options panel.
I tried the Warp function, and it did scale it, but the issue I am having is that the part I am working on is a 2D pie slice of a circular feature with some cutouts in it. When I warped it, the OD/ID are not diametrical anymore. They become more conic. I couldn't tell just by looking at the model, but when I measured it, it doesn't give me a diametrical value, just a curve length which tells me that it's not scaling properly in my model.
Yes, good that you checked. No that you mention it, I remember that the warp function can be less than exact. I just tried it on a simple cylinder, and while it remained cylindrical, the diameter scaled from 100 to 149.995 when I applied a scale factor of 1.5. But it seems like you found a solution, anyway.
Warp function did scale my model, but unfortunately, it didn't warp properly. I responded to this in a post a little further down if you're interested in seeing my response. Appreciate the help!
Unfortunately I don't have the Mold extension. Sounds like that would have been a great option! Appreciate the information/help!!