PDA

View Full Version : Problem path code to S post



Steve Manthey
12-20-2008, 06:28 PM
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
12-21-2008, 08:57 AM
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
12-21-2008, 12:18 PM
Darinbee...Thanks for your help! That did the trick.

Regards,
Steve

Steve Manthey
12-21-2008, 01:23 PM
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
12-22-2008, 01:07 AM
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
12-22-2008, 02:03 AM
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.

Excelmachine
12-22-2008, 02:53 PM
"SEQNO


SEQNO/k,INCR[,m[,n]]

k Is the starting sequence number.

m Is the incremental value.

n Causes sequence number output every nth block.

This is the default condition assumed with k,m,n=1.



SEQNO/k

Generates a sequence number k for the next block only.



SEQNO/0

Causes sequence numbers to be same as .INC and CL record numbers.



SEQNO/OFF

Terminates sequence number output.



SEQNO/NEXT

Generates the next block as an alignment block with the address selected by the Configuration Tool in the sequence number.

Related Commands:

PLABEL/OPTION,30"

From SPOST help menu. Maybe try using SEQNO/OFF? And yes, Surfcam forum here seems pretty dead, specially compared to Mastercam's. Which could mean that Surfcam is easypeesy to use and Mastercam is difficult or that user base of Surfcam is really small.

Steve Manthey
12-22-2008, 07:59 PM
Excelmachine...Thanks a lot for the info!

I gave my test program a shot after work tonight and I was disappointed. The tool path was real jerky...almost like it read a line stopped, then went on to the next. G9 is an "exact-stop check" and at first I thought maybe I had that in there causing this. I checked and there are no G9's. Here is a sample of my program:

O1000
T13 M06
G54 G90
S1459 M03
G00 G43 Z3.1 H13
X.956 Y0. A-148.355
Z3.03
G01 Z3. F5.
G93
G01 X.979 F326.087 A-143.79
X.9951 F326.831 A-138.865
X1.0048 F314.342 A-133.511
X1.0083 F279.942 A-127.384
X1.0046 F359.909 A-122.627
X.994 F395.84 A-118.458
X.9765 F409.97 A-114.776

blah,blah,blah

G94
G00 Z3.1
M6 T13
G91 G28 Z0
G28 Y0
%

Anyone have any ideas?

Steve

Cammotion
12-23-2008, 09:56 AM
Excelmachine...Thanks a lot for the info!

I gave my test program a shot after work tonight and I was disappointed. The tool path was real jerky...almost like it read a line stopped, then went on to the next. G9 is an "exact-stop check" and at first I thought maybe I had that in there causing this. I checked and there are no G9's. Here is a sample of my program:

O1000
T13 M06
G54 G90
S1459 M03
G00 G43 Z3.1 H13
X.956 Y0. A-148.355
Z3.03
G01 Z3. F5.
G93
G01 X.979 F326.087 A-143.79
X.9951 F326.831 A-138.865
X1.0048 F314.342 A-133.511
X1.0083 F279.942 A-127.384
X1.0046 F359.909 A-122.627
X.994 F395.84 A-118.458
X.9765 F409.97 A-114.776

blah,blah,blah

G94
G00 Z3.1
M6 T13
G91 G28 Z0
G28 Y0
%

Anyone have any ideas?

Steve

Steve, I've had this problem before with Fadal machines, and it was because it wanted a G8, which made the controller "look ahead", and not do a line at a time. We were getting the jerky toolpath as you describe. I edited the post to put the G8 in, and no more problems with the Fadal. Haas machines don't seem to have this problem. It sounds like your Mazak needs the G code for this. Perhaps some one can enlighten us on which code your machine needs. Good luck.

Excelmachine
12-23-2008, 12:52 PM
I agree with Cammotion, I also used to run a Fadal and G8 made the countours a lot smoother. I now run an Excel with a Fanuc 21M controller and a G8 doesn't do anything on this controller. The rest of your code doesn't ring any alarms with me, although I am more used to G54 G90 being in the same line with your X,Y and A location.

Steve Manthey
12-24-2008, 01:19 AM
Thank you both for your replies. Yes, the G8 thing was the very first thing that entered my mind. I too had this experience with a Fadal. Mazak doesn't use G8. I might give it a try anyway...worse thing that can happen is it will alarm out and not work. I didn't have any time to play with this problem today, but I really need to resolve this.

Steve

Excelmachine
12-24-2008, 12:59 PM
I'm not familiar with a Mazak but I know that some machines use custom G codes for certain things. I remember using a 4th axis on a Fadal and one of the things we did for the code was always have it spit out the code for the air brake release even if we weren't using the brake.
I also just checked my Fanuc 21M manual and there is a code called G64. The manual states that this is the cutting mode. Some of the comments in the manual say "Once specified, this function is valid until G61,G62 or G63 is specified. The description for this code is stated as, " The tool is not decelerated at the end point of a block, but the next block is executed." G61 being exact stop mode, G62 automatic override for inner corners and G63 for tapping mode. I have never used this command in the 3 years I have been running this machine and we do a lot of 3D surfacing.
If you can find your Mazak manual, maybe check their G code list for anything referencing inverse time or 4th axis moves? Maybe try running your post without any 4th axis moves and see if it acts the same way?

Steve Manthey
12-25-2008, 06:00 AM
Yesterday afternoon I figured out what was going on with that jerky toolpath. It was the brake on the A axis being applied at every move. I just added an M46 and smoooooooooooooooooooooth as silk. Kinda funny, this morning I read your post Excelmachine....You nailed it! I appreciate your input.

Steve

Steve Manthey
12-25-2008, 09:35 PM
This is going to drive me over the edge!!! I'm getting a few things figured out, but as I'm looking a little closer at my program I am finding out that the toolpath is 2.5" above the part. I drew my part flat, then did a "wrap cyclinder" and wrapped the part to a 1.5" radius. I posted it with the 4 axis Spost I'm screwing around with (for days) and my rapid approaches and final depth on "Z" are 2.5" above the dang part. I'm looking at my "File Option Generator" and can't see anywhere that would cause this problem. Any ideas?

Steve

Cammotion
12-26-2008, 11:20 AM
This is going to drive me over the edge!!! I'm getting a few things figured out, but as I'm looking a little closer at my program I am finding out that the toolpath is 2.5" above the part. I drew my part flat, then did a "wrap cyclinder" and wrapped the part to a 1.5" radius. I posted it with the 4 axis Spost I'm screwing around with (for days) and my rapid approaches and final depth on "Z" are 2.5" above the dang part. I'm looking at my "File Option Generator" and can't see anywhere that would cause this problem. Any ideas?

Steve

How about your tool length offset? Or were there any numbers left in the controller from another job concerning that tool number? Where is your xyz zero? Simple things, but I've had them mess me up before.

Steve Manthey
12-26-2008, 12:56 PM
Nope...no tool length offset issues. "Z" is at the center of the part on the "A" axis.

I finally ditched the UNCX file I was using and tried another. All of a sudden I don't have that weird 2.5" above the part issue. I messed with this crap 20 hrs yesterday and 5hrs this morning. The more I mess with this stuff, the more complicated I realize it is. I found out that I need to have a UNCX01.pxxx and a UNCX.fxxx file with the same "xxx" number in the Post Lib file. These are the files that the Surfcam PST file calls up to define which post processor is to be used. What I found interesting is after you post a program, another UNCX file is created in the Post Lib file, It's UNCX01.sxxx What is odd to me is when you look at both of these UNCX.s and UNCX.p files, they look indentical. Another weird thing I noticed is when you make a change in the Optional File Generator, this messes up the UNCX.s file. I kept a copy of the UNCX.s file on my desktop and then after I changed the Optional File Generator I replaced the one in the Post Lib file.

For some of you experts out there, this is probably simple stuff. Being self educated in the computer world, I'm really struggling with this. Any input or advise is greatly appeciated.

I'm going skiing now...
Steve

sinderal
02-13-2009, 01:31 AM
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
02-13-2009, 07:47 AM
Thanks for your reply!
Yes, this machine supports G93 and the "A" axis lock and unlock commands. Can you help me?

Steve

sinderal
02-15-2009, 01:48 AM
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
02-15-2009, 06:47 AM
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
02-15-2009, 10:10 PM
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.

Steve Manthey
02-15-2009, 10:26 PM
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:SURFCAMVelocity3INC2APT" -w -5 -I "%p%n" -O "%p%N.apt"
ChDir "C:SURFCAMVelocity3SPOST"
Delete "%p%N.EIA"
Command "C:SURFCAMVelocity3SPOSTSPOSTM" "%p%N.apt" 2380 "%p%N.EIA"
Task "C:SURFCAMVelocity3editNCeditNC" "%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.


1. Our $ervice contract has run out.
2. I have that figured out.
3. The problem is I didn't draw the geometry at Z2.5" yet the toolpath was way above my part...I did finally figure that problem out too.
4. I'd be happy if 75% of my requirements were met at this point...

Soooooooo, I'll take your suggestion and ask for help...