[Steve Manthey]

I'm hoping someone can help me out here...
I am trying to get a 4 axis post working with Surfcam for our Mazak 510C.
I have been messing around for hours trying to figure this all out and I'm stumped. I aquired two files for the S post and can't seem to get them put in the right place to work when I click on the "post" button in Surfcam. The files I have are:
Uncx01.p2380 and Uncx01.f2380. I found several locations where there is a PostLib folder and I'm not sure which one to put them in. I messed around with this and changed the path in the PST file to:

BeginPost 4 Axis Default:1
PostItem MAZAK NEXUS 510
Status Display all posts in postform.m
ChDir "C:\SURFCAM\Velocity3\SPOST"
Delete "%p%N.NCC"
Command "C:\SURFCAM\Velocity3\SPOST\MPOSTWIN" "%p%n" 2380
Task "C:\SURFCAM\Velocity3\editNC\editNC" "%p%N.ncc"
EndPost

I have something messed up, and can't figure it out. Could someone shed a little light on this?

Thanks,
Steve

[Darinbee]

You have modified an Mpost PostItem instead of an Spost

Make sure your UNCX files are in your C:\SURFCAM\Postlib\Spost folder

Note, the INC2APT switches my not be correct for your Post

Try this instead.

PostItem MAZAK NEXUS 510
Status MAZAK NEXUS 510
Command "C:\SURFCAM\Velocity3\INC2APT" -w -5 -I "%p%n" -O "%p%N.apt"
ChDir "C:\SURFCAM\Velocity3\SPOST"
Delete "%p%N.NCC"
Command "C:\SURFCAM\Velocity3\SPOST\SPOSTM" "%p%N.apt" 2380 "%p%N.ncc"
Task "C:\SURFCAM\Velocity3\editNC\editNC" "%p%N.ncc"

[Steve Manthey]

Darinbee...Thanks for your help! That did the trick.

Regards,
Steve

[Steve Manthey]

Well, I can post a program now, but I'm not seeing any "A" axis moves in the program. I'm not sure if the UNCX files are any good for 4 axis milling though. I got them from Surfcam a few weeks ago. They said they were "public domain" and they may need to "contact your reseller for manipulation of this post if you need it changed". I sure would like to be able to do this myself, rather than be at the mercy of technical support. Our maintenance contract is up so we're screwed as far as help from Surfcam.

Steve

[Steve Manthey]

Well, I messed around with this stuff all day and I have an understanding of how to modify MPosts. In the POSTFORM.M file you make your changes. As far as the Spost goes, I'm totally confused when I look at the UNCX files. It looks like there is an "s", "p", and "f" file with the same preceding number, but when you open the file, it's just an assload of numbers that don't make sense to me. I played around with the Option File Generator and was able to iron out my "A" axis positive and negative degree stuff. I don't want ANY sequence numbers in my program and I was able to get rid of all but the one at the first tool call. I also would like to be able to use G93 (inverse timing) for "A" axis work. Would anyone know how I can achieve this? Will it require a different UNCX file? Where exactly is the G93 command handled?

Any help would be appreciated.
Steve

[Steve Manthey]

I feel like I'm talking to myself here...LOL

I did a little more digging and figured out where the G93 inverse timing is handled. I think I have a working post now! I still didn't figure out that sequence # problem though.

[sinderal]

1. Does this machine support G93 for 4 Axis?
2. Does this machine have the Lock/unlock M-code for the A Axis (Like M43....)

[Steve Manthey]

Thanks for your reply!
Yes, this machine supports G93 and the "A" axis lock and unlock commands. Can you help me?

Steve

[sinderal]

Hi steve,


1. Maybe you did the wrong "Wrap on Cylinder", since your flat geometries drew at 2.5" and programed according to 2.5", how about the "Wrap on Cylinder" parameters setting? You maybe got wrong Z value for your toolpath! What the Z coordinate value and Wrap Coordinate in Wrap Mapping?

That why your actual cutting Z is Z3.

2. Anything wrong in the Spost file Uncx01.P2xxx, Uncx01.F2xxx? except you want to output M46 to unlock you A Axis?

Let me know, what you want to correct?

Send me your scprt file and Uncx01.pxxx and Uncx01.fxxx which you used for that machine, if you want me to help!

[Steve Manthey]

Hi sinderal,

I appreciate your response! I actually have the wrap thingy figured out...this is a message I posted in another forum and what I need help with:

Attention: Mazak 510C owners

--------------------------------------------------------------------------------

I was wondering if someone could help me out. I wasn't able to get much help in my last post, so I'll try this. If I were to supply a Surfcam 4 axis drawing, could someone with a Mazak 510C and a Matrix control post it, and send the EIA program back to me? I am looking for a usable template for setting up my post processor. If someone would have a 4 axis post for the above, what would it take to get a copy? I'm not looking for anything free, I just want to get this machine capable of 4 axis work.

Steve

[sinderal]

Hi Steve,


1. Why you need to modify the Uncx01.P2380 and UNCX01.F2380 by yourself and don't want to ask your Surfcam local dealer to help you? I think it is easy for your local Surfcam dealer to modify for you.

2. If you want the output of NC program w/ EIA extension, just edit the surfcam.pst as

PostItem MAZAK NEXUS 510
Status MAZAK NEXUS 510
Command "C:\SURFCAM\Velocity3\INC2APT" -w -5 -I "%p%n" -O "%p%N.apt"
ChDir "C:\SURFCAM\Velocity3\SPOST"
Delete "%p%N.EIA"
Command "C:\SURFCAM\Velocity3\SPOST\SPOSTM" "%p%N.apt" 2380 "%p%N.EIA"
Task "C:\SURFCAM\Velocity3\editNC\editNC" "%p%N.EIA"

3. Please make sure your "wrap cylinder" are correct.
From your post, you drew geometries at Z2.5 and program it then wrap on R1.5 cylinder. and your cylinder center is Z0. --- If above are correct, then you should keyin 2.5 for the Z coordinate value in Wrap Mapping. Otherwise, you get wrong Wrap Cylinder Tool Path.

4. Even someone have the same 4 Axis Mazak 510C, I don't think his post could 100% meet your requirement. Maybe the Rotary Axis mounting is different and then direction is different.

So, you should dry-run ( if the XYZA value are correct) on your machine and check the program and manual modify then go back to modify your post or ask someone to help.