C-Axis "turning" with side of endmill?

[justchips]

Hey guys,

 

Does anyone know of a way to get Mastercam to output C-axis rotation to "TURN" a contour with an endmill?

 

Thanks for any help. I couldn't get morph to do it

 

I want the code to look like this...

 

a0.c0.

g1 y-1.5

c360.

y-3.

[jlw™]

You could use a contour path with axis substitution and use polar coordinate output.

 

Do you want the end mill to be turning or just skiving? I don't think that'll work.

[mkd]

more info would help, like what machine you are talking.

 

mill turns have turning mode or milling mode not both. at least mine doesn't.

?

[jlw™]

Judging by the snippet of code I'd say he wants polar milling.

 

If you have the 5 axis paths you can use one of them for the same output.

[JMahon]

That's definitely doable on the mastercam side. How you go about it will depend on your machine and if you have 5 axis in mastercam.

[jlw™]

Can you upload a file? Make a simple contour path with what you want.

[#Rekd™]

Yes just use C-Axis contour.

[justchips]

Sorry I fell off the earth for a few hours...I need to jog in to a point of a circle with spindle turning say 1/2 inch endmill in the y or x axis and than rotate c axis turns 360 plus a little...this is a table table trunnion machine... Cublex 35 but we don't want to use a turn tool...

 

Thanks for any help possible...

[justchips]

Yes just use C-Axis contour.

C axis contour?

[justchips]

Judging by the snippet of code I'd say he wants polar milling.

If you have the 5 axis paths you can use one of them for the same output.

Yes polar milling with tool centerline parallel to the c-axis centerline (a0.)...

[Steve Hattori]

Justchips, do you have Camplete for the Cublex? If so, Camplete has a function that will turn any 2d milling op into a C-axis milling with X or Y fixed in space, so it runs like a C-axis contour- polar milling...

[Craig-B]

Is it anything like this? 

 

https://youtu.be/CscXtn49oR8

[JMahon]

Upload a file n I'll shoot u an example in the morning

[justchips]

Justchips, do you have Camplete for the Cublex? If so, Camplete has a function that will turn any 2d milling op into a C-axis milling with X or Y fixed in space, so it runs like a C-axis contour- polar milling...

Steve, this is what I want. I'm just getting up to speed on camplete. Right now I can verify no collisions in simulation and post g-code in the software from my mastercam NCI code. I have some documentation to read tonight. Can you point me in the right direction?

 

Is it anything like this? 

 

https://youtu.be/CscXtn49oR8

 

Yes I believe thats the machine and that IS BADASS...hopefully I can get that tool!!!!  

Upload a file n I'll shoot u an example in the morning

I don't have a file... I drew a 3 inch circle xform copy in z and also extruded a solid. Than i tried to do what Steve described IN Mastercam.

[justchips]

Upload a file n I'll shoot u an example in the morning

I would really appreciate it if you could show me a toolpath that would output this code !!! polar milling using  x/y to lead in than c axis to cut. Thank you so much for any help!! Everything I've done puts the tool perp. to the wal not parallel to the wall that outputs c-axis move 

 

Thanks for helping a young buck out!!!

[JMahon]

You on x9?

[Guest]

I suppose I could be wrong here but unless a post for a 5 axis mill has this option coded into it, I believe the post will always choose a 3 axis(X, Y, Z) first.

 

Polar output for C axis is built into lathe posts but not mill posts that I am aware of by default

[jlw™]

I suppose I could be wrong here but unless a post for a 5 axis mill has this option coded into it, I believe the post will always choose a 3 axis(X, Y, Z) first.

 

Polar output for C axis is built into lathe posts but not mill posts that I am aware of by default

 

 

I am using all Postabillity posts so mine have it, I just assumed mcam generics would output, apologies if i'm wrong - still new to mcam myself.  If your machine supports polar coordinate interpolation you can get the rotary motion with the same old "linear" code by adding a G12.1 after your G43 line and the G13.1 at the end.  I've only seen this capability on 5 axis machines tho, never tried to use it on a 3+1 setup.  Do you have a 3 ax machine with a rotary positioned vertically or are you trying this in a trunnion machine?  You need to take a peek at your manual to see exactly how to activate it.

 

You'll likely have something like this (if memory serves):

 

position

G43 Z line

G17XY

G12.1

motion code

z retract

G13.1

 

Been some years since I used it so search for polar coordinate interpolation in your manual.  Maybe that'll get you closer.

[Guest]

 

I am using all Postabillity posts so mine have it, I just assumed mcam generics would output, apologies if i'm wrong - still new to mcam myself. 

 

 

Custom post......that assumption of base posts having the ability is incorrect.

 

So this is going to be VERY dependent on what is being used for a post for that machine.

[justchips]

Yes X9 ... THE MACHINE is a CUBLEX 35 with Siemens 840

[justchips]

I suppose I could be wrong here but unless a post for a 5 axis mill has this option coded into it, I believe the post will always choose a 3 axis(X, Y, Z) first.

 

Polar output for C axis is built into lathe posts but not mill posts that I am aware of by default

Yes this is what I'm experiencing!

[Guest]

Yes this is what I'm experiencing!

 

What post processor are you using?

[justchips]

An mpmaster post modified for 5-axis post. But for the CUBLEX, I'm using NCI Code to CAMPLETE.

[justchips]

At this point it would be nice to be able to code this way to the robodrills...

[Guest]

If you are going to expect the code right out of the Mastercam post, you are going to have to get some custom post work done.

 

"assuming" that is nothing you know how to do, it's not a simple task, you will want to get with your reseller and let them know what you need.

 

They may suggest instead of post work, just purchasing a custom post processor.

 

MPmaster available through IHS is not a 5 axis post, 4 axis only