PDA

View Full Version : Trouble with Post for Prototrak



Stile2
07-06-2006, 12:01 AM
Everytime I generate a post for use on a Prototrak the Z's are all positive. The ProtoTrak wants to use the top of the part as Z0.0000 and into the part as negative Zs.

How can I change the post to look at the top of the part as the Z0.0000 and into the material as negative Z?

this is from a post that works (from another CAM)
%
O0000
N1 G0G17G40G49G80G90
N2 M6T2
N3 G0G54X-0.0501Y-0.3984
N4 G43Z2.H2
N5 G00 X-0.0501 Y-0.3984 Z2. (Z2.0 is tool change position)
N6 Z0.1167 (Safe distance from the part)
N7 G01 Z-0.0833 F150.0 (Milling the part)
N8 X0.1507 Y-0.4014 F300.0

Here is from your post processor
%
OTest Block
N1 G21
N2 G40 G54 G80 G90
N3 M06 T1
N4 S4000 F300 M03
N5 G43 H1
F20000
N6 G01 X-0.219 Y4.253
N7 Z6.454 (the ProtoTrak barely has this amount of movement in Z)
N8 G01 Z6.000 F300
N9 Y0.000 Z5.250 F300




Thanks

Keith

turmite
07-06-2006, 10:10 AM
Keith,

I am not Joakim but I'm willing to help it possible. First off do you position your parts in Rhino where your machine needs them, with the top of the part being at z0.00? Have you checked your starting position windows for the three different axis when you postprocess the code? If you are not doing this, try those and see if it makes a difference. You can also go to your madcam folder and open the post processor to see if the ++++ moves are in the post.

Mike

Stile2
07-06-2006, 10:38 AM
I have managed to "trick" MadCam into posting correctly, but the other CADCAM programs that I have seen and used, you don't have to trick it.

For example, OneCNC, when you go to post, asks where the top of the part should be. It would be nice if MadCam did the same.

I have already changed the Post Processor to work in Inches, and got rid of several extra things in the processor. I have to say the language in which the post processors are written are the most understandable I have seen.

Keith

lakeside
07-06-2006, 11:20 AM
I ran Bobcad with a prototrak dpm mx3 controller ran great no issue other than upload load time baud rate is slow

Stile2
07-06-2006, 11:36 AM
Here is the beginning of my post after I moved the part below the x-y plane, so that the top of the part is at Z 0.0000. The first G00 move is to Z 2.0000 X 0.0000 Y 0.0000 for a tool change.

Let me know what you guys think. Does it look like your posts?
Onegative2
N1 G20
N2 G40 G54 G80 G90
G00 Z2.0000 (In position for a tool change)
G00 X0.0000Y0.0000
N3 M06 T1
S2000 F10
F100
N4 G00 X-1.2164 Y-1.4990
N5 Z0.1250 (Rapid move to safe distance from the part)
N6 G01 Z0.0000 F10
N7 X-1.5000 Z-0.0500 F10 (Mill into the part)
N8 X1.5000
N9 X1.5068 Y-1.4979

Thanks
Keith

lakeside
07-06-2006, 11:44 AM
attached you will find an excel worksheet sent to me by southwestern ind. maker of prototrak The sheet list all G-codes for prototrak

lakeside
07-06-2006, 11:46 AM
you will need a .(period) after your F10 (F10.) if not feed will be F1.0

Stile2
07-06-2006, 11:56 AM
Thanks for the G-Code list, it is a little more detailed than the book I got with the Prototrak retrofit.

Keith

turmite
07-06-2006, 04:15 PM
Keith just remember that Onecnc is a lot more $$ and many people writing the code (I'm assuming here). Joakim is a self employed mold and die maker that also writes code for Madcam. I know for a fact that lots of changes are coming in Madcam and have been in email contact with Joakim on a regular basis.

I have a very unique setup for a machine and use Mach2 for a controller. I explained my need to him and he did me a post that works just like I want it to. Email him directly, but be prepared to wait a couple of days. I sometimes have to but realize his situation and am prepared to wait.

Mike

Stile2
07-06-2006, 04:41 PM
Please understand I am very happy with MadCam. I think it works great and is easy to use. I just have this one issue. What I really want to know is how to rewrite the post processor in order to make it do what I want. I am a teacher and if I learn this I can teach my students.

turmite
07-06-2006, 06:17 PM
Keith have you opened the particular postprocessor? Now I know very little about programming and therefore the reason I did not write my own post.

Here is the post:

//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Prototrak
*FILE_EXTENSION*
dnc
*FILE_DEST*
c:\postfiles\
*FILTER*
0.001
*OUTPUT_WIDTH*
4
*OUTPUT_DECIMALS*
3
*SCALE_X*
1
*SCALE_Y*
1
*SCALE_Z*
1
*AXIS_1_CHAR*
X
*AXIS_2_CHAR*
Y
*AXIS_3_CHAR*
Z
*CUTTER_REFERENCE*
TIP
*RAPID*
F20000
N"lnbr" G01 "x" "y" "z"
*END_SECTION*
*RAPID_APPROACH*
N"lnbr" "x" "y" "z"
*END_SECTION*
*RAPID_RETRACT*
N"lnbr" G00 "x" "y" "z"
*END_SECTION*
*APPROACH*
N"lnbr" G01 "x" "y" "z" F"feedz"
*END_SECTION*
*FIRST_CUT*
N"lnbr" "x" "y" "z" F"feed"
*END_SECTION*
*CUT*
N"lnbr" "x" "y" "z"
*END_SECTION*
*TOOL_CHANGE*
N"lnbr" M06 T"toolnr"
N"lnbr" S"speed" F"feed" M03
N"lnbr" G43 H"toolnr"
*END_SECTION*
*TOOL_STOP*
N"lnbr" M09
*END_SECTION*
*PROGRAM_START*
%
O"pgmnr"
N"lnbr" G21
N"lnbr" G40 G54 G80 G90
*END_SECTION*
*PROGRAM_END*
N"lnbr" G80 M09
N"lnbr" M30
%
*END_SECTION*
*LINE_START_NUMBER*
1

Maybe someone can give you some help as to how to modify it. I would also try several of the different post on the same part to see how they output code. If you find anything that looks like what you want go to the Madcam folder and open that post along with the one for your machine. The differences will be evident pretty quick......I think.

My best reccomendation though, is to contact Joakim directly and tell him your problem and what you are wanting to do with the post......teach.

Mike

JOM
07-06-2006, 07:34 PM
Hello Keith,

If you want to cut the model with z=0 at the top of the part, it’s just like Mike said, place the model in Rhino with z=0 at the top of the part. It is also very easy to move the model together with toolpaths in Rhino before posting. Please let me know if you would like to change something in the Prototrak postprocessor and I will customize it for you.

Joakim

Stile2
07-06-2006, 08:09 PM
Moving the model is what I figured out. that method is working well, thanks

I have already modified the Post Processor with help from the ProtoTrak book, and it seems to be working. I have to say that the Post Processor language in MadCam is infinitely easier to understand than some other CAM programs I have seen.

Thanks for your help,
Keith

lakeside
07-07-2006, 02:53 AM
looking at the info (from turmite post) change file extension to .CAM unles you run in DNC mode then file extension must be .DNC

//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Prototrak
*FILE_EXTENSION*
dnc (change to .CAM)
............

Stile2
07-07-2006, 10:21 AM
I actually changed the extension name to .gcd which is one of the formats the new Prototrak reads. The Prototrak book mentions the .cam, but I am not sure what it involves. I'll give it a shot though. thanks

Keith

lakeside
07-07-2006, 11:40 AM
.cam was a file extension prototrak used with the MX3 series and o;der controll instead of .TAP or .CNC

Stile2
07-07-2006, 12:01 PM
The prototrak book says that the .cam file will be converted into prototrak events. I will have to investigate further, probably in the prototrak forum (if they have one).

lakeside
07-07-2006, 12:09 PM
When a .CAM file is loaded in controller it stander EIA format when you save or read the file at the controller then it looks like there events here a sample of a cam program that was saved as a .mx3 format
PN2 G20;
G130 X0.0000 Y0.0000;
G131 Z-0.2000 XM-2.0000 XN7.0000 YM-2.0000 YN5.0000 ST=11111;
N1 G108 XC+0.0000A YC+0.0000A ZR+0.0300A ZE-0.1450A R0.3125 DR1 NP04 FC0.0020 F10.0 FZ4.0 FF10.0 D0.2500 T01;
N2 G105 FE0001 LE0001 XO+2.3000I YO+0.0000I ZO+0.0000I ZF+0.0000I RE002 D0.2500 T01;
N3 G105 FE0001 LE0002 XO+0.0000I YO+1.7500I ZO+0.0000I ZF+0.0000I RE001 D0.2500 T01;

turmite
07-07-2006, 12:54 PM
Hi Keith,

I talked with Joakim this morning and we discussed the postprocessor for a good bit. What would your thought be on a wizard type postprocessor editor?
I think some might call this conversational.

Mike

Stile2
07-07-2006, 01:23 PM
Wow! That would be really cool! I am a noobie at this whole g-code thing. I am learning fast but it is a pretty steep curve. I am all in favor of a wizard type editor. Let me know if there is anyway I can help. I am more than willing to be the guinea pig tester guy.

Thanks
Keith

turmite
07-07-2006, 05:05 PM
No......not a gcode wizard, but a postprocessor editing wizard. Sorry if I wasn't clear on that. BTW if you want conversational??wizard programming take a look at the mach3 controller. It has several wizard's built in, plus a dxf to gcode cam called Lazycam. I don't know anything about your machine but you might be able to get all of it to work together.

The thing I have discovered is that each time I fire up Madcam, I learn something new that I did not know the program could do.

Mike

Stile2
07-07-2006, 08:04 PM
Sorry, I understood a post processor wizard. But I meant that if I had that I could use it and see what happens to the g-code and learn it that way. I think that would be great!

SeaSchell
09-03-2006, 06:37 PM
.gcd is to run file as an NC file., (does NOT convert although you can view in Setup, Toolpath) .cam converts to Trak conversational language, (although it doe NOT like some standard G/M code stuff)

Stile2
09-03-2006, 08:11 PM
thanks
I actually figured it oout a while ago just didn't post. I can pretty much do what ever I want at this point using .cam programs

Thanks
Keith

lakeside
09-05-2006, 11:22 AM
if you choose to run dnc just change file extion from .cam to .dnc I had the same issue when I first started with a prototak

trakman
12-02-2006, 10:50 AM
ProtoTRAK .cam files are G code files generated on a CAM package. When read into the TRAK control (any ProtoTRAK control with a color monitor), they are converted to ProtoTRAK's own conversational language and the program resides entirely in the system's memory. The program may then be edited, previewed and run. .cam files will run in G61 (exact stop) mode, meaning a definate stop at each not-tangent entity union. Larger G code files (generally programs for 3D contours over 1 MB) may take too long to convert from G code to conversational. Those types of files are better suited to be run as .gcd files.

.gcd files are also G code files generated on a CAM package. These files run in DNC mode, meaning the pass through the system's memory as opposed to residing in memory like a .cam file would. .gcd files run in G64 mode, meaning free cutting mode, and flow through non-tangent entities. .gcd files allow any size program to be run as you would with any sized DNC program.

You do not have to rename .cam file to run them as .gcd files. To run a .cam file as a .gcd file: Select program in/out, open, highlite your file, tab down to open as and select gcd - then select open file. Beats renaming a long list of existing .cam files or .dnc files from previous versions of the ProtoTRAK control.

Hope this is of some use.

TM