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