I am creating a forging that will be chemically milled, which means that .010 will be taken off of all surfaces, I need to expand my model to allow for this reduction. I know that I can scale the model, for thermal shrinkage and what not, when I use the scaling feature and type in .01 not all of the surfaces changed correctly, it expands the entire model by 10% not .01, does anyone know how to accomplish this?
: "Shaun T" wrote : it expands the : entire model by 10% not .01, does anyone know how to accomplish this?
Select all the surfaces/quilt and offset by .01 (or -.01?), but how to do this (button pushes) depends on the rev of Pro/e you are using.
David Janes
Thanks alot David, that was a good idea I already tried it and it didn't work, what happened is the geometry was to complex and when all sides were offset .01 some geometry overlapped and blew up. It isn't a bid deal. What I am going to do to fix it is when I cut the die on the CNC in my tool path parameters I am going to set the stock allowance to a negative .005, which will be a total of .01 after both sides of the die are made.
Shaun
The old way (in v2001) was the do a surface copy of the entire part and then offset/copy the surface the required amount of the c/m offset, and then create a protrusion using this surface.
In WF we now have edit/thicken. You click on the model to select a face, right click to select 'solid surfaces' and create the surface copy. Then use edit/thicken to create a protrusion with the offset.
The new edit/thicken seem to be more robust that the old surface copy/offset, and 'sometimes' will even 'swallow' small features or edge patches OK.
BTW, I also design forgings in pro-e. (Oh death, where is thy sting?)
:-)
How do you add 'shrink'? Do you have the mold design module? (I don't)
I was go> I am creating a forging that will be chemically milled, which means
: > Select all the surfaces/quilt and offset by .01 (or -.01?), but how to do this : > (button pushes) depends on the rev of Pro/e you are using. : >
: > David Janes : : : Thanks alot David, that was a good idea I already tried it and it : didn't work, what happened is the geometry was to complex and when all : sides were offset .01 some geometry overlapped and blew up. It isn't a : bid deal. It actually is a big deal. One of the things that offsetting surfaces helps with is precisely the kind of part anomalies that you found. And it is an anomaly when surfaces intersect and thus fail. It means that there are walls on protrusions that are so thin that they will disappear when this much stock is removed. Unless you mean to put holes where none are designed or turned flats (say, at the top of a rib) into sharps, this should tell you that the model exceeds minimum wall thickness somewhere. Something that should be checked on, don't you think.
: What I am going to do to fix it is when I cut the die on the : CNC in my tool path parameters I am going to set the stock allowance : to a negative .005, which will be a total of .01 after both sides of : the die are made. : Horrible, awful idea, resist the temptation to take this foot-shooting, "easy" way out. You are only making trouble for yourself down the road. If anyone else is trying to work with your programs, this is a good way to yourself marked as a .... well, there are so many unpleasant names, I can't think where to start. So, my advice: stick with the surface offset method. It has the advantage of being widely used and recommended so you look like a pretty sharp and sophisticated user if you practice this; it is a recommended way of checking the manufacturability of models -- it's a free byproduct so why not take advantage. And you won't make any enemies by faking out your fellow programmers.
One other possibility for error in offsetting surfaces needs mentioning: model accuracy. If set too low, offsetting can challenge Pro/e's ability of correctly offset surfaces, especially when small patches are formed. Move the relative accuracy setting one more decimal place to the left and try it again.
David Janes
Chris, I do have the mold mod so it is really easy to add or minus shrinkage. If you do not have the mold mod it is still really easy to add shrink, all that you have to do is have your .prt open, then click on modify and scale model, when i use this i scale it 1.009 because we have found for the type of Ti and the temps we are running at we get .009 inches of shrink per inch. The scall model makes every thing larger by .009inch per inch. This is the same as in the mold mod but the mold mod allows you to pick 1/(1-s) or 1+s and it also allows you to use different values for different directions.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.