c axis face groove

[Clarence L Cook]

I need some help.

 

I have an Amera-Seiki TC-2L with live tooling. I have a family of parts that have various face grooves ranging from .015" to .090" width with ODs on the grooves from .095" to .940". I am ramping the appropriate sized endmill to make the face groove to the desired depth.

 

The problem that I am having is that as the OD of the groove gets larger, the code expands dramatically. The smaller grooves were defining the end points 180 degrees apart and .001" deep, which is OK but not ideal. While the largest groove defines the end points 5.373 degrees apart and from .0001" to .0002" deep.

 

Ideally, the code would be the depth of the groove and the total degrees to make the groove, ie Z-.03" C1152.

 

I am in the process of modifying the mlmaster for X4 to get the code right for my machine.

 

I have tried a little of the cordial deviation in the c axis face contour operation, but I got some X values which are not appropriate.

 

Any help would be appreciated.

[crazy^millman]

I would look to using Axis sub for this. It might give you cleaner code.

 

 

HTH

[Clarence L Cook]

I am looking at the Rotary Axis Control and the Axis substitution is grayed out. I only have the option of Y axis and C axis. My lathe is only XZC. The geometry that I am picking is an arc of the appropriate OD.

[Clarence L Cook]

The code that I am getting is a linear move, not a circular move, because it is just two points, Z and C. I am thinking that something is breaking up the linear moves to some distance. That would explain the differences due to the size of the arc.

[Clarence L Cook]

Does anyone have any ideas? Is there a parameter that I am missing?

 

Thanks.

[Ron Branch @ Verisurf]

Write the code out yourself should be pretty straight forward. Should be something like this.

 

G00 X2. Z.05 C0.

G1 Z-.2 C3600. F120.

G1 C360.

G00 Z.05

 

That would do what you are looking to do. Sometimes you just have to throw in the towel and just get the job done.

 

HTH

[Clarence L Cook]

It posts out all the stuff I need. There is just a lot of it.

 

I am currently modifying by hand (I was half afraid I my have to stick with this route) just as you suggest.

 

What I think I want, I might not be able to get. I was hoping that I was missing a parameter setting.

 

Thanks for the reply Ron

[Ron Branch @ Verisurf]

Well I would ask did you try this using a C axis toolpath or just a regular mill toolpath? There is a difference.

[Clarence L Cook]

I am using the c axis toolpath.

[mayday]

have had issue's with c axis paths in X4. use mill paths instead

[chris m]

Does the machine have coordinate system conversion? Might be easier to just use G03 X Y Z I J K and let the machine figure out the C/Z relationships

[Clarence L Cook]

MayDay. I will try the mill tool paths. I haven't used them in a lathe before.

 

Chris. The machine is a '95 machine with the Fanuc 0T control. When we purchased it a few years ago, it didn't come with any of the Fanuc manuals, so I don't know if it has the conversion capabilities.

[chris m]

With a Fanuc 0, I am guessing not, but I could be wrong

[Clarence L Cook]

That is my guess also.

[kennebec]

Just a thought: we often use Misc #4 set to 1 and output G12.1 and G13.2 Polar Mode on and Off respectively...

[Clarence L Cook]

I just went to the machine and tried G12.1 in MDI mode. The control will not accept a decimal with the G code.

 

I am going to try some of the prior suggestion tonight. I will share what I find out.

 

Thanks for the help.

[JMWorks]

May try G112 instead

[GoetzInd]

Try G112 and G113.

Misc Int. #4 set to 1 in mplmaster