Machsupport Forum
Support => Downloads => Post Processors => Topic started by: dba on October 29, 2006, 11:30:49 AM
-
Here's the post pro i made for solidcam 2006.
U just have to unzip the 2 files in ur /solidcam/GPPtool folder.
Feel free to comment it.
DB.
-
Thanks for that, I will upload it to the new post pro section. http://www.machsupport.com/cam.htm
-
IMPORTANT! I just started with SolidCAM and found out that the M3 and M4 have been switched around in this post processor! already broke a tool because of this.
-
dba,
Thank you for this post pro. I am just starting with mach3 and SolidCam and I must say, it works great! I am trying to let my milling machine work in 4 axes (X-Y-Z-4_axis_around_X) but it seems the 4_axis_around_X does not work... I think this is becouse the mach3 post-pro does not have the 4th axis implemented. Is it possible for me to do something like that ?
@ debos,
What doe you meen by that the M3 and M4 are switched around and is this possible to solve easily?
Greatings from Holland!
-
spindle direction is inverted (M3 = Clockwise, M4 = Counter clockwise) So when you chose the option CW in SolidCam, your spindle will turn in the wrong direction
It is easy to fix withe a texteditor, like notepad. Maybe it's fixed already (?) ???
Also greetings from Holland! ;D
-
Debos,
Are you sure they are inverted in solidcam or is it the way your spindle is wired or your the way your outputs are set up in Mach? I have a couple of ideas to help with this in any case. Is solidcam the only way you generate code or do you use other cam packages as well? If you type in M3 in mdi, which way does your spindle turn?
Brett
-
I know for sure. I use all sorts of CAM programs, so I noticed it by reading the generated gcode (did that after the crashed tool ::) ) It's wrong in the post processor code
@start_tool
if only_xyz eq false
if tool_direction eq CW then
mcode = 4
else ; CCW
mcode = 3
endif
call @gen_nb
{'S'spin:integer_def_f, ' M'mcode}
call @gen_nb
{'M8'}
endif
endp
You see, it sais CW mcode=4 and CCW mcode=3. I editted it, now everything is fine.
-
Yup, that'll do it. Glad you got it.
Brett
-
is there a solidcam post processor for 4 axis to work with mach3?
-
Hi
When i make an array (nesting) of my part in solidcam whit the command Transforme ->Translate->Matrix.. Mach3 halts on a line wich starts whit "while"
I've using the mach3 postprossessor.
%
O5000 (SAETREGAARDENMYNT.TAP)
( MCV-OP ) (28-MAR-2010)
(SUBROUTINES: O2 .. O4)
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T1
(TOOL -1- MILL DIA 3.0 R0. MM )
G90 G00 G40 G54
G43 H1 D31 G0 X0. Y-10. Z20. S1000 M3
M8
#21 = 0
WHILE [#21 LT 3] DO 1
(---------------------)
(P-CONTOUR-T1 - POCKET)
(---------------------)
G0 X0. Y-10. Z10.
Z2.
G1 Z-0.2 F330
G3 X0. Y-10. I0. J10. F3000
G1 Y-10.2
Is there any changes that i can do in the .mac/gpp files to fix this?
-
Mach3 has no looping macro commands.
Graham
-
Is there an updated post processor out for Solidcam that has the M3 & M4 issue corrected?
Thanks,
-
here's my version of solidcam post for 2010 /2011 , any problems let me know with an example and solidworks /solidcam files etc and i'll fix
Dave
-
Dave, I've been fighting with my post processor for solidcam (modified FANUC) and came across your post. I think there are few issues. The biggest one is the tool change. When the tool is changed from shorter to longer tool, the longer tool gets rammed down to the previous level and then there is a rapid move to the new XY position where the new longer tool is set to the correct height.
Below is the example of the code that was generated with your post.
My own version of the post does a similar thing with is what I have been struggling with.
Other notes: the 50mm above Zero is not valid on my mill and gives soft limit warning (had to change it to 0), I also work in inches but the post forces mm (changed to G20)
I can send you my design files off line if you want to play with them.
I don't know enough about post processor design and gcode hence my inability to fix the problem. Just trying to get though this tool change problem.
Thanks for your help
%
O5000 (FT44145)
N5 G0 G40 G49 G80 G21 (Initialisation)
N10 G0 G53 Z50 (Return to origin machine & 50mm above Z Zero)
N15 G0 G53 X0 Y0
N20 (Tool n° 2 - Diameter 0.125 D2 H2)
N25 M6 T2
N30 S5000 M3
N35 M8
N40 (D-drill5-T2)
N45 G0 G54 X2.408 Y-0.75
N50 G43 H2 Z0.4
N55 G83 Z-0.845 R-0.021 Q0.14 P0 F15
N60 G80
N65 (Tool n° 3 - Diameter 0.094 D3 H3)
N70 M6 T3
N75 S1200 M3
N80 M8
N85 (D-drill1-T3)
N90 G0 G54 X1.807 Y-1.292
N95 G43 H3 Z0.4
N100 G83 Z-0.381 R0.079 Q0.16 P0 F8
N105 X3.195
N110 G80
N115 G0 G53 Z0 M9
N120 G0 G53 X0 Y0 M5
M30
%
-
ok i'll take a look
the 50mm above is purely a safety issue and can be changed to suit , i'll default it lower to say 10mm
i will also add a second post for Imperial users , to make it easier
regarding the toolchange , i'm not totaly convinced the problem is in the post , this could be attributed to a number of setup situations , although i will look further into this
it's normal when setting toolchangers , to set the longest tool first in tool position 1 reference this to tool offset zero , also make sure any and all tool offsets are zero at this stage , then all subsiquent tool offsets are used and set for tool 2 onwards
this should account for the problem you have .
if you are using tool offsets in Solidcam, then make sure any offsets are zero in mach3 and are not used
you may have a combination of offsets between solidcam and mach 3 , choose which program you want to use and make sure the other application is zero
it's not the first time iv'e been caught out !
Dave
-
updated post files included Imperial version
-
for people using toolchangers and in Sinij Kot finding my deliberate error ! , attached is an update post processor with fixes , it defaults to metric but see included txt file showing changes needed for Imperial
Dave
-
Dave, I really appreciate you talking time to work on this.
Here is my setup: SW/Solidcam 2010, BP knee mill, manual tool changes.
You reminded me about something I read long time ago about longest tool first but since has forgotten about. I actually sort my tools by operation sequence, make life a lot easier for me. This of course means that tools are not necessarily sorted by length. I agree that sorting them by length should fix my problem, but I see that as more of a band aid than "proper" operation. If you designing the post why not make it so that tools don't have to be sorted by length, make it a don't-care.
I would expect tool change to go like this going from tool 1 to tool 2:
G53 G0 G28 Z0 (rapid raise tool 1 to machine Z zero to give most clearance for tool change)
M6 T2 G43 H2 (ATC change to tool 2 apply offset from the table for tool2)
S3200 M3 M8 (start spindle, turn on coolant)
G0 Xnew Ynew Zclearance (offset is applied just before this move and this move brings you to clearance level defined in solidcam)
I am sure my syntax is not proper but I think you can get an idea of what I think would be a safe tool change
This is the new code generated with your improved post
%
O5000 (FT44145)
N5 G0 G40 G49 G80 G20 (Imperial Initialisation)
N10 G0 G53 Z1 (Return to origin machine & 1.0 Inch above Z Zero)
N15 G0 G53 X0 Y0
N20 (Tool n° 2 - Diameter 0.125 D2 H2)
N25 M6 T2
N30 S5000 M3
N35 M8
N40 (D-drill5-T2)
N45 G0 G54 X2.408 Y-0.75
N50 G43 H2 Z0.4
N55 G83 Z-0.845 R-0.021 Q0.14 P0 F15
N60 G80
N65 (Tool n° 3 - Diameter 0.094 D3 H3)
N70 M6 T3 *****************This wants to do a tool change right where the previous tool stooped*****************
N75 S1200 M3
N80 M8
N85 (D-drill1-T3)
N90 G0 G54 X1.807 Y-1.292 **************Makes a move before the offset is applied********************
N95 G43 H3 Z0.4 *********************I think this line should be moved to N70 M6 T3, this way offset is applied before the move**************
N100 G83 Z-0.381 R0.079 Q0.16 P0 F8
N105 X3.195
N110 G80
N115 G0 G53 Z0 M9
N120 G0 G53 X0 Y0 M5
M30
%
By the way, in solidcam under part definition / tool options you can define the tool change position, but it never gets populated in the gcode. I thnk the post just ignore it. I even tried changing default tool change position in MAC file without any change. I would be nice to have this option working, because sometimes I want a specific tool chage location to clear the part when there is not enough Z height available.
Dave, I'll send you my files shortly.
-
I'm using Solidcam /solidworks. Mach3 etc etc.. solidcam MILL operation post is ok using mach3.gpp, but there is only a FANUC.gpp for the TURN operation and during the G code generation I continually get a system 'xc' error and the Toolgpp error.
It will not generate G code.. even on simple straight 'turn' jobs.
If try to configure the mach3.gpp into the TURN post processor Solidcam will error "not correct gpp type '.
Is there a fix for this is or it just me doing something wrong ?
-
Hi Tony,
I use for Solidcam turning MACH30T.gpp and MACH30T.mac.
They are not made by me , but they work with Mach3 and my Emco5 cnc.
They work for me. I found these on the Internet somewhere.
Regards,
Jos
Give it a try,
Jos
-
check your email Tony
yes i am aware of the problems with the fanuc turning post , i am making progress with one , i hope to test more fully during the weekend , i'll post it here once iv'e tested it
but if anyone is willing to also test it let me know .
Dave
-
here's the latest version for milling and included the Turn post processor , both in metric and Imperial
these are work in progress , so first run with care , anything you find let me know , along with any fixes and hopfully we can keep these active and improve as we go
Dave
-
I just wanted to mention that Dave (CNCBasher) spent a ton of time with me last weekend modifying solidcam post to make the manual tool changes more sensible. After hours of work we were able to generate g code which did tool chage perfectly without ramming the tool into the work ;D.
Thank you Dave, I owe you one!
-
Thanks Dave for the post processor. I am using Solidworks 2011 and Solidcam 2010 to Mach 3 to my new Taig mill. I am having trouble with the most recent version of this post processor. I am working in imperial units.
I am getting error codes as follows:
"Line 430: invalid GENERATE statement"
"Line 430: unrecognized statement"
and
"Line 640: cannot initialized GPP tool environment"
I am completely new to CNC and may be doing something simple and wrong. Has anyone run into this error, or know what I may be doing wrong?
Thanks for any direction!
-Wes
-
I am also getting those as invalid.
"Line 430: invalid GENERATE statement"
"Line 430: unrecognized statement"
I'm also generally having trouble with my machine coordinates with solidcam. When I open any soldicam gcode from the standard fanuc or from this post my machine z wants to start at machine 0 rather than at my work offset or work position. To solve this problem I either edit out some lines or set the work position 0 and then restart mach so that the machine coordinates and work offesets are both at 0,0,0
Apart from this I have no problem with the standard faunuc so far. Ive attached the standard fanuc files in the hope that someone might have a look at how to change this and below is the gcode that gets generated out of a generally solidcam fanuc
%
O5000 (F_CONTOUR37_T11.TAP)
( MCV-OP ) (17-SEP-2011)
(SUBROUTINES: O2 .. O0)
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
N1 M6 T11
(TOOL -11- MILL DIA 3.0 R0. MM )
G90 G00 G40 G54
G43 H11 D41 G0 X16.976 Y-9.56 Z50. S1000 M3
M8
(-------------------------)
(F-CONTOUR37-T11 - PROFILE)
(-------------------------)
X16.976 Y-9.56 Z10.
Z-4.553
G1 Z-12.553 F33
G2 X15.712 Y-9.627 R1.5 F100
G3 X21.9 Y-15.894 R-11.075
G2 X22.244 Y-14.284 R1.5
G1 X22.418 Y-14.112
G3 X22.431 Y-11.991 R1.5
G1 X19.621 Y-9.145
G3 X17.5 Y-9.131 R1.5
G1 X17.326 Y-9.303
G2 X16.976 Y-9.56 R1.5
G0 Z10.
X25.006 Y-25.742
Z-4.553
G1 Z-12.553 F33
G2 X25.075 Y-26.811 R1.5 F100
G3 X31.499 Y-29.509 R3.5
G2 X32.665 Y-28.728 R1.5
G3 X24.815 Y-25.432 R-8.875
G2 X25.006 Y-25.742 R1.5
G0 Z10.
M30
%
-
Anyone got a 4th axis post processor?
-
Please if anyone had a 4th axis post for solidcam and mach3 it would great.
ad
-
Please if anyone had a 4th axis post for solidcam and mach3 it would great.
ad
Try with the Fanuc 4th axis. I always erase this:
G90 G17
G80 G49 G40
G54
G91 G28 Z0
G90
M01
see ya
-
Lucas thanks:) Im guess do you mean mean the standard faunc.mac file(because I see no file with faunc_4 or something like that)? I was guessing it was only for 3 axis but now that I open the mac file I can see num_axes = 4. Are you using it with a rotary table?
-
No, the thing is that i have a 3 axis milling drilling machine that i have converted, but in april there is a new syil X6 big table with 4 axis that is arriving to my workshop here, in Argentina. In my workshop i make engine competition parts, and i want to make an inner shape, so that why i need the 4th axis, i dominate the solid cam with 3axis, but i never can do anything with the 4th. So i try with mastercam for solid works, it's great! but i dont dominate like the solidcam. I try for making one camshaft lobe, just for trying, and then i have tried something like that of the inner shape, but it's strange, because every single code the feedrate change, ok nevermind.
What i know about the 4 axis in the solid cam is that yo have to pick the rotary axis (x, y, z) and then you start with the option of the 4th axis. Did you try with milling turning option? because it make the 4th axis option available. But the post procesor didn't work, and the fanuc option is not available. May be with a post pro that recognize the milling turning option we can use the 4 axis.
-
I have had a quick look at the mill-turn but as you say no post is available that I think would suit. There are users using a 4th axis rotary table but I guess they use other cam software:( Ive seen on cnc zone one guy who says he has a 4th axis which I did ask him for and had had no reply. Its such a shame that one of the leading cam packages doesnt provide more clear examples and I also kinda whish the mach3 developers would at least ask the solidcam software makers to push for one as it would increase sales for both products..thats just my opinion though..I have also looked at the example multi side machining and I will at least give it a try when I get to my friends machine again. Anyway I wish the whole thing was more open..Perhaps other users using such mills as the grizzly or bf20l with a rotary table can tell us what works for them.
-
Is there a solution for these messages?
I use SW2010 and Solidcam 2011. The postprocessor is from cncbasher above.
It is not possible to generate a G-code so the SC is in fact useless for me.
thanks.
Thanks Dave for the post processor. I am using Solidworks 2011 and Solidcam 2010 to Mach 3 to my new Taig mill. I am having trouble with the most recent version of this post processor. I am working in imperial units.
I am getting error codes as follows:
"Line 430: invalid GENERATE statement"
"Line 430: unrecognized statement"
-
Hey everyone,
I just downloaded the postprocessors for solidcam, but when I load the toolpath in mach3, I get the tollpath inside of erratic G2 and G3 movements that shouldn't be there. I've tried other postprocessors but any of them gave me the exact toolpath as it's shown on solidcam screen.
Can anyone help me? I don't know if it has something to do with solidcam itself and can't be modified or if it has something to do with the postprocessor.
I even tried different machining strategies to see if it was something related to that, but the results are the same.
I've attached the gcode, so you can understand me easier. The blue lines (toolpath in mach3) are the correct code and the pink are the wrong movements that shouldn't be there.
Please, any expert, give some help!
-
No expert by any means, but :
Gen. Config.
Select Inc. IJ Mode.
See if that helps
-
To be clearer,
On the Mach screen, top menu, left.
Config. / Gen. Config / IJ Mode - Inc.
:)
-
then click REGEN. to regenerate the toolpath and the magenta circles/arcs should go away.
-
THANK YOU SO MUCH, MAN!!!
You are an expert for sure!
If you don´t mind to help me with something more, I have a question about the scaling factor.
Everytime I run a gcode, my X axis goes automaticaly to scale factor of -1.000. Do you know if this is related to the gcode? Is there any configuration in Mach3 that I could disable it?
In fact, what is it for? I couldn't notice any difference...
Thank you
-
-1.000 would produce a mirror image on that axis. If the part was symmetrical, it would make no difference. Your cam must not be putting that in the code cause I dont see it in the code you sent. It might be in your config, initialization string ? ? ?
You can use G50 to cancel all scaling, in the beginning of your code.
Post your XML (copy to desktop and rename first) if you wish, might see something there.
-
From the manual:
6.2.2.4 Scale
Scale factors for any axes can be set by G51 and can be cleared by G50. If a scale factor
(other than 1.0) is set then it is applied to coordinates when they appear in G-code (e.g. as X
words, Y words etc.) . The Scale LED will flash as a reminder that a scale is set for an axis.
The value defined by G51 will appear, and can be set, in the Scale DRO. Negative values
mirror the coordinates about the relevant axis.
The G50 button executes a G50 command to set all scales to 1.0
-
:)
Did you build this machine yourself ? Is it factory built ?
Reason I ask, there could be macros or plug-ins involved with the scaling.
Also, this, for your reading pleasure.
Cheers,
Russ (novice) ;)
-
Thank you again.
I've built it from scratch, every single part. It is being a great adventure. Everything modeled in Solidworks.
I'll post the XML tomorrow after I get back to my working place.
There are some brains, like the ones for the aqua screen and for the MPG Pendant.
I'm using the smooth stepper too, but I don't think its plugin is causing this.
You said about the G50 to cancel the scaling and I tried editing the Gcode, but as soon as the program jumped to the line below the scale on the X axis turn on again, on an eye blink.
I'll load a XML from the last week and see what happens.
Best regards
-
Don't know what was causing the scaling, even if I commanded a G50. I updated the postprocessor, so the max feed and rapids doesn't cross my machine limits.
Mach3 is working OK now.
Thank you for your help Overloaded.
Now, I'm fighting against another problem. My router doesn't accept feedrate updates during gcode running. Neither feedrate overwrite.
Some times, in the gcode, there are some Fx... commands,like ones on toolpath linkage, and my machine servos jerks when these commands lines runs.
As if they were jammed or something, giving just small "punches" instead of the right movement.
Any clue how to solve this issue?
-
Hello using SC 2010 to Mach 3 on taig mill and keep getting the z going down to like 200mm? I tried all 3 Posts on this thread and the Fanuc as well. I checked the drawing and don't see any OD points etc..?
-
a pic of the mach 3 tool path preview?
If anyone can help me I would really appreciate it, thansk in advance :)
-
I think your best bet would be to contact your salesman where you bought the program as that is part of their job to set you up with a proper post processor for Mach 3.
Dave
-
A guy im going to school with is going to sell me his complete laptop with the software on it. It is nice but for the price he wants if i cant find a PP that will work I will just look at bobcad. For what I do I dont need anything crazy. It is nice though. His shop switched to Mastercam.
-
Is there a solution for these messages?
I use SW2010 and Solidcam 2011. The postprocessor is from cncbasher above.
It is not possible to generate a G-code so the SC is in fact useless for me.
thanks.
Thanks Dave for the post processor. I am using Solidworks 2011 and Solidcam 2010 to Mach 3 to my new Taig mill. I am having trouble with the most recent version of this post processor. I am working in imperial units.
I am getting error codes as follows:
"Line 430: invalid GENERATE statement"
"Line 430: unrecognized statement"
I'm also getting the same error, did anyone ever get a post processor working for solidcam,??
-
Hi - I had the problem also - there is a small typo in the mach3.gpp file. You can simply open the file with a text editor and go to line 430.
This line has an extra hyphen at the end:
{'T'tool_number,' M' mcode,' D'tool_number,' H'tool_number'}
just delete that so you have:
{'T'tool_number,' M' mcode,' D'tool_number,' H'tool_number}
and your problem should be solved.
I have also attached the revised imperial version of the post here.
if you need metric post - just follow the instructions above.
-
Well spotted bscandanavia, thanks for posting the details. ;)
Tweakie.
-
I also have a problem with postprocessing for my EMCO fCNC turn. Can you please send me turning MACH30T.gpp and MACH30T.mac
-
I also have a problem with postprocessing for my EMCO 5 CNC turn. Oldraven can you please send me turning MACH30T.gpp and MACH30T.mac
-
My MACH3 postprocessor use for G02 and G03 R instead of I and K definition and I have wrong radius on that command. This happens only in Mach3 controler for my lathe (in CIMCO is OK). Also X coordinate is in - and have to be in + (this I solved in notepad with REPLACE). Can someone halp me with this?
-
I solved the problem. After postprocessing for turn with tool in front of piece you must replace X- with X+ and G02 with G03 and G03 with G02. After that works fine.
-
Hey,
I did put some effort myself into the SC mach post :
https://youtu.be/brfYdzQtdQs
https://youtu.be/uzifjFm5B8s
https://youtu.be/uzifjFm5B8s
https://youtu.be/uzifjFm5B8s
I've set up a github repo (https://github.com/teodoryantcheff/SolidCam-Mach3-Post)
Any feedback and comments welcome.
PS -- the backplotter used in one of the videos is the one from the free hsmexpress. Really nice program.
PS2 -- Since I don't have a licensed SW nor SC I go to a friend of mine, who works at a shop and they have "real" machines -- HAASes and so on, and he let's me play with their software. So it's a painfully slow process... :) I'm yet to build my own machine.