Reply with QuoteI see you're here too. Good. This is a better place to discuss madCAM issues.
Can you post a sample of good code (something small)? It shouldn't be that difficult to create a post for you.
Dan
Madcam postprocessor for Vickers PC2100 on tree vmc750
Curious if anyone on the forum can help. I recently purchased madcam 5 educational and have been emailing madcam for a postprocessor for a tree PC2100 Vickers controller on a machine I'm working on but have not received a reply from them. Tried couple different times now.
I'm anxious to tryout a few things but without post processor I'm getting no where short of running another post processor and reviewing and editing everything..... not my idea of a lot of fun but possible.
So is anyone running madcam on pc2100 controller?
Similar Threads:
I see you're here too. Good. This is a better place to discuss madCAM issues.
Can you post a sample of good code (something small)? It shouldn't be that difficult to create a post for you.
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hi Dan,
Just for clarification... you just looking for a small existing program that runs on the machine?
if you can find a post for fanuc 0m you can edit it to what you need , like for g3, g2 fanuc would use a "R" for the radius and the pc2100 uses "P"
most everything else is the same
They do have a Fanuc OM post, if I'm not mistaken some of the code related to fixture locations are different as well but I'm just getting used to this controller, some things are nice on it, it does have a fanuc translator built in as well gonna go bore myself with the manual a bit...:
//MadCAM_POST_2003-12-10
*VERSION*
1.0_031210
*FILE_NAME*
Fanuc 0M
*FILE_EXTENSION*
nc
*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
G1"x""y""z"
*END_SECTION*
*RAPID_APPROACH*
"x""y""z"
*END_SECTION*
*RAPID_RETRACT*
F20000
G1"x""y""z"
*END_SECTION*
*APPROACH*
G1"x""y""z" F"feedz"
*END_SECTION*
*FIRST_CUT*
"x""y""z" F"feed"
*END_SECTION*
*CUT*
"x""y""z"
*END_SECTION*
*TOOL_CHANGE*
T"toolnr" M06
S"speed" F"feed" M03
G43 H"toolnr"
*END_SECTION*
*TOOL_STOP*
M09
*END_SECTION*
*PROGRAM_START*
%
O"pgmnr"
G40 G55 G80 G90
*END_SECTION*
*PROGRAM_END*
G49
M30
%
*END_SECTION*
*LINE_START_NUMBER*
1
Yes, a small program that runs without issues. Then a post can be reverse engineered to replicate that code.
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Here is a simple one for doing some spot drilling and drilling
N10 G1
N20 G70
N30 G90
N40 M6 T8
M8
N50 G0 X0 Y0 Z1
N60 G82 x2.5 y1.25 Z-.125 R0 S600 M3 F25
N70 X3.75 W1
N80 M6 T9
M8
N90 G81 X2.5 Y1.25 Z-.5 R0 S2500 M3 F25
N100 X3.75 W1
M9
M2
here is another for rigid tapping:
N20 G70
N30 G90
N35 M8
N40 G84.1 J1 X2.5 Y1.25 Z-0.606 R0 S200 M3 F15.38
N45 G84.1 J1 X3.75 Y1.25 Z-0.606 R0 S200 M3 F15.38 W2
M9
M2
madCAM doesn't support drill cycles yet. That's being worked on. You can drill point-to-point, but tapping is not possible yet.
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
ok let's try something else then:
about as simple as it gets, most of mine are at this point, just facing off an edge
T4 M6
S1800 M3
G0 x-1.0 Y0.25 Z-0.060
G1 X9.0 F12.0
Y0.6
X-0.5
Y0.8
X9.0
M5
M2
Here is another that does rectangular pocket generated on the "resident assistant programmer" (built in):
:G97 G94 G70 G90 G0 X0 Y0 Z3 S2000 F50 M3
G25.1 G90 X0 Y0 U8 V4.5 O0 R0 Z-0.04 ,R0.5 Q1 J0.25 K0.02
P50 I0.01 W1 F50 S2500
G0
G0 G90 X0 Y0 Z10
M2
The first example is useful. Is that complete? No O lines or % to start or finish? No safety lines?
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Yes that works as is. Probably one of the first ones I did on it, nothing to brag about... Everything else is holes, tapping, etc.. Surfacing/profiling/pocketing stuff is where I want to go, reason for madcam. Programming holes and tapping at control is not really a big deal so not really a train wreck that madcam doesn't do it out of the box, I wanted it more for complex surfaces.
machine as I mentioned earlier does have built in Fanuc translator, 850sx, and 950mc. There is a section with tables in programming manual showing Fanuc compatibility for different codes. Many are the same but biggest difference is use of "words" in work coordinate systems and others. for instance G54 is H1. Inch and metric designation also different. G20=G70 and G21=G71.
I can probably copy and scan some of this section of programming manual if that would be helpful. Let me know.
Thanks for your help in advance!
As much info as possible would be helpful. I can't promise I will get to this immediately, but I will try over the weekend.
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
A2100 G-M code and fanuc translation info from manual
Dan,
Trying to attach scanned copies of programming manual. 2 sections, one deals with g and m code references the other is the fanuc translation section.
had to do second post for second pdf file..
You purchased an Educational license. There is no support included in these kind of licenses, so don't expect that e-mail support is rated as a high prio thing.Originally Posted by trelos_zoi
If Dan is looking into it I'm sure you'll get something useful. Did you try any post processor? Usually some posts are close enough to get running after a few mods.
I took a quick look at the attached information and it seems the majority of differences from Fanuc are related to cycles and arcs (neither which are supported in madCAM yet). I'm going to take a kick at the can and do some mild modifications to my Trak post and then give that a try on the machine. It will be for metric (G71) so be aware you may need to change that if you don't use metric (to G70 for imperial). Not sure what file extension you need so I'll make it .nc. You can alter that if need be. I don't see any provision for fixture offset (G54, G55 etc.) so I'll leave that out. It possible that G92, G92.1 is the fixture offset, but it's not clear to me that that is what is meant by "Position set" but it very well may be. We can add that later if that is in fact your fixture offset code.
Also, I'm not sure what your rapid feedrate is, so the post report may not be accurately reporting the rapid time. My value is 10000 mm/m so you may need to do something with that (especially if you work in inches, which we never do). Same comment on toolchange times. Time a toolchange and adjust that value to match your machine. Don't worry if you skip this step, it's only for reporting purposes. It won't affect the code.
Let me know how close this is. We can tweak it once you tell me what doesn't work for you.
Dan
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Hey Dan,
Thanks for feedback and post. Sorry for slow response on your hard work but had a death in the family so been out of pocket for a few days.
I'll give it a try this weekend and let you know how it goes.
Thanks Again!
svenakela,
thanks for reply I wasn't aware of that fact or overlooked it one and is understandable at the reduced pricing etc.. Would of been nice to have just gotten a quick email stating something to that fact from the guys at madcam, no response is a bit frustrating.
True, agree with the responding. Too much work I guess.
