C-AXIS LATHE

[Mickey@acceltool]

OK, I have been programming lathes for a short time now and I am having problems with C-AXIS stuff.

When I c-axis face mill flats on my diameter and then go to drill a c-axis hole on those flats, the holes will not land on the flats I just machined. How can I control this in Mastercam X7 or from a machine config? I will attach a example file.

 

Thanks

CAXIS.MCX-7

[DODGERFAN]

It looks like you may want to use some other views when you are doing the drilling.

You also can program just one hole and do a transform rotate 2X's at 120°

[crazy^millman]

With C Axis toolpaths you have to remember the movement to cut a flat starts at one angle and then goes to a finish angle for the flat. If you only have lathe and not mill then you cannot use the method I am thinking which is Planes and Milling toolpaths not C axis toolpaths. Will still be a C axis toolpath because in the axis substitution you will tell it C Axis. From what I can see looks right what kind of a difference are you seeing on the parts?

[Mickey@acceltool]

The holes are not landing on the flats that I cut. I have a lathe with live tooling. It drills the holes in between the flats. The milling and holes are not indexed the same to each other. How do I get the posted code to cut the part correctly as I program it and as you see it on the screen?

 

Dodgerfan!!! What other views??? Please explain!

[DODGERFAN]

I'll do my best here. I'm not to savy with c axis so these are just shots in the dark. (disclaimer)

You can choose a solid face and make that the view for you path.

Go to planes, view by solid face then choose the flat as your "new view" give it a name like "view for flats" and program it from there.

[Mickey@acceltool]

I program from one plane and my machine is supposed to index the part accordingly. I use only one plane/zero when programming the lathes.

[DODGERFAN]

But with a C axis your no longer just in lathe mode.

[K2csq7]

It drills the holes in between the flats.

 

So, relative to the flats, the holes are off 60°?

Or are they off 90°?

[Mickey@acceltool]

30 degrees.... I guess my big complaint is I just don't know how to control where these features are cut. I just rely on the software to do it for me and most of the time it is wrong. What am I not getting here?? I get that I am in a "milling" mode but how do I control it??

Sorry if I sound frustrated.

[DODGERFAN]

 

Sorry if I sound frustrated.

That is so not necessary here. You are preaching to the Choir when it comes to frustration.

That's what this forum is for, to lessen the frustration. When this forum cant help we will suggest beer.

[AEP]

I pulled in your file and used C axis cross drill and everything worked perfectly for me, whenever I cross drill, I tend to use the cross drill tool paths, select rotary axis control to C axis, and you should be golden.

[Glenn Bouman]

I agree with using cross-drill, you will notice the C-axis drill shows the holes out of position also.

[K2csq7]

I've been spoiled with multiaxis...

Can anyone explain the difference between C axis drill and C axis cross drill?

TIA!

[Mickey@acceltool]

That was it. C-axis cross drill in "X6" shows an example in the toolpath type dialog box as if you were drilling off of center as if you had a "Y" axis on your lathe, so I would never used it because I don't have a "Y" axis. I have always used c-axis drill. In X7 in the toolpath type dialog box it shows the C-axis cross drill..... drilling on center line of the part (totally opposite) of X6. FML!!!

 

So from now on I will only use C-AXIS CROSS DRILLING.....I have fought with this for a long time...

 

Thanks for your help!!!!1

[Mickey@acceltool]

PLEASE SOMEONE EXPLAIN!!!

[Chris Rizzo]

C-axis cross drill lets you select c OR y axis on the rotary axis control page of the toolpath. It has regular linking parameters that "make sense".

 

C-axis drill basically is using axis substitution, where on the rotary axis control page you need to enter a diameter of your part, which is ADDED to all the linking parameters. Not as easy as regular cross drill, you always are having to think through what the dia of a particular feature you are on...

 

An alternate way to go is use regular milling toolpaths, with the rotary axis control page set to C-axis. It takes an understanding of the view-manager and t/c planes a bit but there are a few parameters that aren't avail in the c-axis toolpaths, but you have access to in mill. (not to mention the fact that you can use any and all the mill toolpaths!) The best way to set up the correct planes for full blown milling toolpaths is using the c-axis utility, a little hidden gem. You will find it under the Mill Toolpaths, the very first thing at the top of the list. It's pretty easy to figure out.

 

hth