[moldcore]

I’ve got a concave surface to cut with a shell mill that’s open on two sides that are opposite each other. When I do Z rough with a Zig Zag cut it wants to cut around the perimeter at each depth. This a total waste of time that adds 50% to the cut time and I can’t seem to find a parameter to make it stop. Man I hate Surfcam!

[Billetgrip]

Is your extents box bigger than the perimeter?

[mariojl]

I’ve got a concave surface to cut with a shell mill that’s open on two sides that are opposite each other. When I do Z rough with a Zig Zag cut it wants to cut around the perimeter at each depth. This a total waste of time that adds 50% to the cut time and I can’t seem to find a parameter to make it stop. Man I hate Surfcam!

There is more than one way to control the tool so it won’t cut on the outside perimeter.
If you create a profile equal to the outline of the part, and use it to set your Material Type to “Top Profile” (or Bottom Profile); in this way the tool will be contained and won’t be cutting on the outside perimeter. Of course the plunge must be set to either ramping or helical, no way to get into the material using those two openings on the sides.
Other way is to create an outside surface which represents the actual stock material and then set Material Type to “Surfaces”, the system will cut all that’s between both surfaces. Something to watch for; both surfaces ( inside and outside) must be looking at each other ( “surface orientation”)
Mario

[moldcore]

There is more than one way to control the tool so it won’t cut on the outside perimeter.
If you create a profile equal to the outline of the part, and use it to set your Material Type to “Top Profile” (or Bottom Profile); in this way the tool will be contained and won’t be cutting on the outside perimeter. Of course the plunge must be set to either ramping or helical, no way to get into the material using those two openings on the sides.
Other way is to create an outside surface which represents the actual stock material and then set Material Type to “Surfaces”, the system will cut all that’s between both surfaces. Something to watch for; both surfaces ( inside and outside) must be looking at each other ( “surface orientation”)
Mario

It's not cutting the out side. Just going around the inside like a finish cut but it's not cutting anything, just air. This part is big so it wastes a full minute to go around cutting air, even the open ends. Maddening. The interface in Surfcam is so stupid that it doesn't remember all the setting if you want to change a parameter or a combination of them. If you didn't write them down you can spend all day trying get out the kinks of a program. Auto Rough using a planer cut would work but you don't have full control of where it plunges, not good if you're using a shell mill. I'm using Surfcam 6 BTW. I refuse to spend and support this worthless POS any longer.

[Billetgrip]

It remembers the parameters if you set up the defaults like you want them. Are you using the classic Z Rough or the current?

[moldcore]

There is only one Z Rough in V6 that I’m aware of. If there is a new one, I apologize for my ignorance and lack of updates the past two years. The parameter I’m talking about is the Material Type. This box should in the main menu and not open after. For example, If something is not working right, I will want to see what option I chose previously. The way it is now I have no Idea what one was chosen unless it was written down. The same goes for “Check Surfaces”. If you want to re-cut the same surfaces but just change the offset amount you have to reselect all those offset surfaces again. That used to be part of the main menu and if you changed the offset it would recalculate without reselecting. Worked great for setting up a semi finish program.

I’ve been using this program for close to 20 years so I think I know it pretty well but this Z rough with a shell mill has got me puzzled as to why it’s cutting so much air. It’s basically a 12” radius 7 inches deep and 14” wide, open on each end. I had the same problem cutting a convex surface before this.

[Billetgrip]

I'm not at a computer now but there is a check box in the options menu to use classic 3D milling.

[moldcore]

Oh yeah, THAT check box. I had checked it long ago for another operation and had forgotten about it. This opens up an entirely different dialog that I'll have to do some research into. Thanks for pointing that out.

[moldcore]

The new Z rough worked great. I could actually take bigger Z steps because the cutter wasn’t engaging at full width on the first pass. My only complaint was that there seemed to be too many options and some of the defaults were a bit unrealistic but I still have much to learn about the newer version. Of course that Material Type window still opens separately making it difficult to review your settings later. Oddly, time wise it was about the same if you use the same depth of cut. Now I have to shovel 175 lb of aluminum chips into barrels, turn the part over and machine about 100 lbs more only that side has islands, should be fun. Thanks for you help guys, I may start liking Surfcam again, NOT. I don't use the Z rough very often, as you can tell, because most of what I do is pretty small and everything I do is one-of-a-kind.

[moldcore]

I'm getting plunges where there shouldn't be. Is there a setting that would prevent the plunges inside the profile using a 2" shell mill?

[Billetgrip]

Are you using the HSM version now? Start from outside box checked?

[moldcore]

Yes to both questions.

[moldcore]

It does start from the outside, only jumps over the raised area in the middle and plunges into an unfinished area that it didn't complete prior. It also does a full tool engagement in some areas that I don't like. Any Ideas would be appreciated. I can send a model if you'd like.

[Billetgrip]

I've drawn what you've described and tool pathed it with a a 2inch and shellmill. The only thing I changed from default was checked Start from Outside, Refine passes, Plunge Ramping and changed Maximum Feed Between to 0.010. Mine isn't showing it plunging into any material. I'm not sure what to tell you.

[Billetgrip]

The Max Feed Between should fix the full width cut.

[moldcore]

Try putting 4 posts in the corners and 2 on each side in the middle so there is 6 posts total. The top of the post are at Z zero. it's open between each post.with a simple convex surface below that is -1" below Z zero at it's highest point. With Max feed set at .010 I'm still getting full width cut.

[Billetgrip]

Oops. ...thought we we're still talking about the concave surface.

[Billetgrip]

Sort of like this?

[moldcore]

Yes that would be what it looks like, only it's mush longer with flats towards each end between the posts. I gave up with the newer Z Rough and used the old version. Less Efficient but it didn't plunge inside the material lines. What parameter settings did you use? I may be doing another one of these soon.

[Billetgrip]

Attachment 241564Attachment 241566Attachment 241568