Need Help!- Simple Wrap Around Dia. Plz-HELP

[MassiveTool]

Hey guys,

This is my first post here but I have been reading this discussion forum for quite a while. Everyone here seems pretty helpful so maybe you can help me out.

This seems pretty simple but for some reason I cant get MasterCam to cooperate with me.

Please help, What am I missing here ?

Basically,
1)I am trying to wrap a line scale around a .980 diameter.
2)Engrave the line scale on a 4th axis (w/ a 3 Axis VMC w/true programmable 4th axis).
3)I have the line scale drawn linear (calculated on, pi * .980dia / 25units ) (every 14.4deg.).


Currently
I am engraving the numbers flat. Meaning, “engrave line /number” index 14.4deg. “engrave line/number” index, etc., etc. but the depth is different because of the contour of the .490rad. only by about .002/.003 but this makes quite a difference when engraving as you all know.

My question,
How can I wrap this around a .980dia. , and engrave it on a 4th axis following the .490rad. keeping the “Y” axis stationary on C/L and use the “X” and 4th.

Thanks in advance.

[chuy]

Not really sure how to do it in X, but in 9 there is a Rotary Axis tab in the tool parameter page. there should something like that in X..just tell it the diameter and you be good...pretty easy. You can even backplot it.click on the substitute axis rotation it'll let you see what your doing.

[Donkey Hotey]

What kind of machine are you using? Haas has an option for rotary axis substitution that does exactly what you want here.

You change a setting in the control that substitutes Y axis for rotary axis movements, input the 'diameter' to use and it does the rest. You post the path as if it's flat, the Haas wraps it around the part.

[g30u0w0]

Did you say what kind of machine you are using? I don't remember. I do this a bunch on a lathe. Use the roll function in mastercam and specify the diameter to roll the geometry around. You will know if you did it right if your geometry still looks flat but your toolpath looks rolled around part. Other thing to keep in mind is where you draw the flat geometry. If c axis orientation is important you must start the geometry at x0 otherwise rotationally it won't start at C0 when posting. PM me if you still have problems I can help you.
G30

[g30u0w0]

sorry I guess you did say you were using a VMC. MEss with the roll function and axis tab under parameters. Let me know how it goes

[MassiveTool]

Originally Posted by chuy Not really sure how to do it in X, but in 9 there is a Rotary Axis tab in the tool parameter page. there should something like that in X..just tell it the diameter and you be good...pretty easy. You can even backplot it.click on the substitute axis rotation it'll let you see what your doing.

Thanks Chuy....Found the tab, I now have somthing that seems to be working. Looks good in verify. The only issue is there is some wierd geometry that has now been generated. I think it has to do with the way I have the WCS / C-plane set.

I drew this geometry in Auto-Cad then when I opened it in mastercam I set the C-plane zero. This did not change the mastercam WCS. Untill now the applications that I use Mastercam for this has never been an issue and the tool path works just fine.

If I zoom way out, and press F9 I can still see the original default WCS. I need to move this, or move the work to it.

Not sure, this may run ok the way it is. Gonna have to post it and take a look.

But thank you very much, I'm headed in the right direction as to understanding this. (Sigh of Relief)

[MassiveTool]

Originally Posted by Donkey Hotey What kind of machine are you using? Haas has an option for rotary axis substitution that does exactly what you want here. You change a setting in the control that substitutes Y axis for rotary axis movements, input the 'diameter' to use and it does the rest. You post the path as if it's flat, the Haas wraps it around the part.

Thanks for your reply Donkey.

It's on a Fanuc O. It doesn't have this type of conversation. Would be real handy tho.

Thanks again.

[MassiveTool]

Originally Posted by g30u0w0 Did you say what kind of machine you are using? I don't remember. I do this a bunch on a lathe. Use the roll function in mastercam and specify the diameter to roll the geometry around. You will know if you did it right if your geometry still looks flat but your toolpath looks rolled around part. Other thing to keep in mind is where you draw the flat geometry. If c axis orientation is important you must start the geometry at x0 otherwise rotationally it won't start at C0 when posting. PM me if you still have problems I can help you. G30

Thanks for the input G30, I didnt think about this. I am also gonna look into that. I do have a lathe with live tooling. This may be a better option. Still need to understand the VMC 4th totally as I have several pcs already cut off. Then I'm gonna work on that to get rid of the 2nd Op. I'll PM you as soon as I get this VMC figured out. Thanks for the offer of help and your repy.

[chuy]

since it's a rotary axis than make your work zero has to be at the center of the diameter will work perfect! and when you post it it will have positve #'s in the Z..looks like you got it..