Lathe- C-axis scribing/engraving

[pantherprogrammer]

Good morning to all.

I, like most, am not real thrilled w/ the lathe side of MC, but you gotta do what you gotta do. My question is, when programming a scribe/engraving on a round portion of a particular part what do you use? Example-I must scribe the part number on a .460 diameter on the part. The particular machine I am using only has a C-axis. I normally create a surface of the diameter and X-form project onto the surface. I then use c-axis cross contour to achieve the scribe. The backplot/verify looks fine, but when I post, the code is not correct. After some hand edits I can make it work. I have tried the surface finish project and c-axis contour and these particular paths generally give me issues. What kills me is the fact that I can program an intricate complex aircraft part for our horizontals with few issues, but when trying to do a simple lathe part I am ready to pull my hair out and go work at Home Depot. So again, what do you use? Any tips or tricks that have worked well?

 

Thanks.

 

Dustin

[JDowe]

Sometimes the projected geometry is not

clean enough to write a toolpath on

- create the geometry flat write a contour

toolpath and roll it around the dia.

[Scott Lundin Shopware Inc.]

Use the C-axis contour operation with rotray axis control set to axis subsitution. Draw the letters flat and chain them flat.

 

 

[Josh T™]

Scott nailed it!

 

I do this all of the time but I typically engrave on the face of a round part and engrave around an arc. If your post is setup with G112 (Fanuc) then this will work great and not take up huge amounts of code.

[Scott Lundin Shopware Inc.]

G112, love it.

[pantherprogrammer]

Thanks guys, I gave that a shot and it looks to be good. One other question, the G112-is that only compatible on FANUC controls? We haven't been able to get that to run on our mori's? Or maybe I need to look at the post?

 

Thanks again guys.

 

Dustin

[Scott Lundin Shopware Inc.]

I had a Mori-Seiki SL-20 M/C lathe and a couple ZL-150 SMC lathes. Used G112 on all of them very successfully. It was a few years ago but if I remember I had to have the post changed a little for the start up and ending code. M46 engage C, M47 dis-engage C, G28H0??????? Cant remember exaclty. You turn on G112 using the misc button and it is one of the misc integers.

 

Edit: now that I think about it, I only used G112 when c-axis milling on the face. I don't know if it works on an OD.

[pantherprogrammer]

Thanks Scott,

I will have my post guy take a look and do a little more research. This is a function I would love to be able to take advantage of.

 

Dustin

[Philcott]

On our Mori G112 (polar notching) is for cutting on the face and G107 is for cutting on the diameter (cylindrical interpolation).

[pantherprogrammer]

PhilCott,

I tried changing the misc integers to output the G107 and it ended up cutting my X depths in half???? It also posted as G7.1. Is this normal?

 

Thanks.

 

Dustin

[Philcott]

My guess is there are a couple of changes that need to be made in the post. I'm not much help in that department but I will say BACK UP YOUR POST before making any changes.

 

Hopefully someone else can take you into the post to make the needed changes.