View Full Version : - a CNC start - need some help gurus. -
http://bcdracing.com/cnc/PIC_0004.jpg
i entered some gcode today. and got it to transfer from my
shop pc.
now the help i need is how do i get gcode from the
mastercamX or solidworks i have?
one green question at a time. this is what happens if you
don't fork over 15k for school kids. :eviltongu
Inclag
07-24-2006, 10:13 PM
It depends on your machine.
At my company we have MatserCam 8 for software, and run it on a Fadal and I believe the other machine we have is a Remington. I know for our machines we program and just export as .NC files either to a linked DOS computer for our Fadal or as .txt for our other machine.
What I do is save my Solidworks files as an IGES and then open it in Matsercam. From there you can save and program your mastercam file and .NC program.
Honus
07-24-2006, 10:16 PM
I'll give a call to my machinist tomorrow and ask him real nice if you can call him directly with all your CNC questions- I'm sure you will have many! He's made a ton of parts for me and is a CNC wiz.
Jerome
i don't think my fanuc controler will use .nc files.
its old and need gcode, i think.
honus, thanks. i posted here not in a mastercam site b/c i knew one
of you guys would like to help me or know of someone who could.
Westy
07-24-2006, 10:29 PM
I know little about Mastercam but the easiest way to get the program into the control is via an RS232 conection runing Procom or similar program on your PC. Actualy Mastercam should have the ability to transfer through he serial port. I forget what kind of control you have, there are parameters that may need to be set to get it to work properly.
Westy
07-24-2006, 10:31 PM
Here is a link I send a lot of people to, pretty much explains all you will need to know.
http://www.machinetoolhelp.com/Applications/RS232Communications.html
LaharDesign
07-24-2006, 10:42 PM
I've been thinking of emailing you about whether you've tamed your cnc rig yet. No advice from me , i've always sent my solidworks models to the pro's. When you're dialed you can mill some molds for me. I'm happy to give you advice on your production mold designs.
yeah, new mold are going to have all bolt holes molded in.
i want to just take them out and bolt them up. super close
with nothing but resin to remove from mold lines.
alex
EVRAC
07-25-2006, 01:29 AM
.nc is typically the extension used for g-code.
After you've got it all planned in mastercam and you have run it through "verify" and it looks good, just post it with whatever generic fanuc or yaznak post-processor work for you. Might take a little experimentation.
What exactly is the question?
Percy
07-25-2006, 06:02 AM
.nc is typically the extension used for g-code.
After you've got it all planned in mastercam and you have run it through "verify" and it looks good, just post it with whatever generic fanuc or yaznak post-processor work for you. Might take a little experimentation.
What exactly is the question?
What he said.
Finding a postprocessor that will talk to your controller is the tricky bit, but if its a common enough controller it shouldnt be an issue.
MikeT
07-25-2006, 08:00 AM
Nately27 and I used .dnc files that he produced through NX I think, and used kwikdnc ( http://www.kwikdnc.com/ ) to transfer the file through RS232 to the CNC machine. I'll forward him this thread so he can maybe help you better
i'll give it a try. thanks for the help.
Red Bull
07-25-2006, 09:27 AM
are you guys speaking english?:o:
atrokz
07-25-2006, 09:52 AM
I had a whole crapload of post processors but you can download a few of the intraweb.
Order of operations:
Design program (solidworks)
converted to
MasterCam (or other maching program) (you can also do the design work in mastercam, and its not too hard)
Converted to Post Processor
send to machine
If you need more detailed help, add me to MSN and I'll see what I can do. I haven't been on the machines for a few months now but I'll see what I can do.
update:
i got it to go across with mastercam's fanuc controler.
ran a simple program but it needs some debuging.
i think i am on my way.......................
I had a whole crapload of post processors but you can download a few of the intraweb.
Order of operations:
Design program (solidworks)
converted to
MasterCam (or other maching program) (you can also do the design work in mastercam, and its not too hard)
Converted to Post Processor
send to machine
If you need more detailed help, add me to MSN and I'll see what I can do. I haven't been on the machines for a few months now but I'll see what I can do.
i like it simple like that, thanks
maybe i'll have somthing to show off later
coma13
07-25-2006, 10:55 AM
any of you experts know any good 3d drawing or CAD type programs for mac or similar plugins for Illustrator for mac?
I'm not needing anything super advanced but i've had some ideas kicking around that i'd like to toy with in a more exact program...
OK, i have got some simple programs into my cnc but its ruining to machine zero to the full extent of my x-y-z @ 10'' each.
but machine is zeroed.
anyone know how to set my machines zero to more centered on my work area?
Sounds like a fun project. I program for a CNC router in Mcam8... but cant really lend any advice here..... wheres buildyourown when you need him??
atrokz
07-25-2006, 12:49 PM
anyone know how to set my machines zero to more centered on my work area?
Not sure what machine you are using but it helps to have a pointer of sorts if you are just looking to get into a general area. For more precise work you need an edge finder, or a indicator.
What controller are you using? I'm used to HAAS, Fadel, and Fanuc (bit rusty on this, as I used it for EDM work only)
OGDMFG
07-25-2006, 12:56 PM
you should have way of using a work offset say G54 for your part offset, make sure in your post processor you have the part using the same x,y and z as your program, just check to see if your program has a return x.0 y.0 z.0 the way I program I like to have the machine come out in y all the way so you do not have to lean so far over , oh and be sure you retract your spindle before you rapid out.
hope this helps
jeremy
its a fanuc, i think i found the line that had it run out there.
now i have overrun my z- down and it will not come back....
i wanted to see my table area
any ideas.
atrokz
07-25-2006, 01:06 PM
its a fanuc, i think i found the line that had it run out there.
now i have overrun my z- down and it will not come back....
i wanted to see my table area
any ideas.
Can you send your G-code program? atrokz at hot...
its a fanuc, i think i found the line that had it run out there.
now i have overrun my z- down and it will not come back....
i wanted to see my table area
any ideas.
On your previous question, it sounds like you're programming with a world coordinate then eyeballing the part zero. Is that correct?
I like to use a local origin, say the center or corner of a block for instance, instead of a world coordinate with an offset. I like to minimize my chances of a crash due to a math error. Takes a little more time on set-ups but worth it for the type of work I do. I also have a safely block inserted before each tool change. Looks like this:
G0 G40 G49 G90 G17 Z0
I'm not exactly sure what you've done here....is the machine in 'alarm'? If that's the case then you need to reset to clear the alarm and then you should be able to zero return the Z or jog it back out of that position.
edit: I reread your question....you should be able to go into the post processor and set the XYZ you want it to finish on. SurfCAM's is pretty straight forward once you find it. I think it's a file called "MPost". My programs take the Z to machine zero, leaves the X at it's last position, and runs the Y to full positive. Here's what my end blocks look like:
G0 Z1.1
G0 G49 G90 Z0 M5
G28 G91 Y0.3319
M02
%
Westy
07-25-2006, 01:43 PM
its a fanuc, i think i found the line that had it run out there.
now i have overrun my z- down and it will not come back....
i wanted to see my table area
any ideas.
You may have hit a hard over travel switch, if so there could be an OT override button on the panel. Ther is also something called a soft overtravel where the position exceeds a value set in the control, you should be able to jog the axis in a manual mode back in the right direction.
EVRAC
07-25-2006, 02:19 PM
To add to what the others heve been saying:
The machine has what is called the "World co-ordinate system" or WCS, these are the machine home position and axes. You need to define the "Part co-ordinate system" or PCS using one of the user definable origins like G54, G55, etc. For x and y you can use the center of your part or a corner or a hole or any other convienient position. For z I would recomend using the top of your workpiece as it makes it easy to see if your cutter is the right height off the part.
Westy's got it right about the overtravel.
o tryed just joging after restart. there is a alarm but i can't clear it till i get the z back in its range.
i have no jog, inc or mpg, it will not move in any axis till the alarm is off.
it is just flashing not ready.
should i take the servo off and turn by hand back in range?
http://www.cnczone.com/forums/showthread.php?postid=148757#post148757
lol
overtravel switch was stuck. i got bcd's fav tool after it and whipped her into shape!
i'l study up what you guys said about wcs tehn i'll bring more problems to you.
here is what i am playing with gcode wise.:
%
O0000(MACHINE_GROUP_1)
(DATE=DD-MM-YY - 25-07-06 TIME=HH:MM - 14:36)
(MCX FILE -)
(NC FILE - C:\PROGRAM FILES\MASTERCAMX\MILL\NC\MACHINE_GROUP_1.NC)
(MATERIAL - NONE)
( T1 | 1/2 FLAT ENDMILL | H1 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
/ N104 G91 G28 Z0.
/ N106 G28 X0. Y0.
/ N108 G92 X10. Y10. Z10.
N110 T1 M6
N112 G0 G90 X-1.0339 Y-.5767 S3056 M3
N114 G43 H1 Z.25
N116 Z.1
N118 G1 Z0. F6.42
N120 X-1.0027 F24.45
N122 G3 X-.3723 Y-.3903 R1.212
N124 G1 X-1.6643
N126 G2 X-1.8929 Y-.2038 R1.212
N128 G1 X-.1437
N130 G3 X.003 Y-.0174 R1.212
N132 G1 X-2.0396
N134 G2 X-2.1371 Y.1691 R1.212
N136 G1 X.1005
N138 G3 X.161 Y.3555 R1.212
N140 G1 X-2.1976
N142 G2 X-2.2267 Y.542 R1.212
N144 G1 X.1901
N146 G3 X.1937 Y.6352 R1.212
N148 X.1901 Y.7284 R1.212
N150 G1 X-2.2267
N152 G2 X-2.1976 Y.9148 R1.212
N154 G1 X.161
N156 G3 X.1005 Y1.1013 R1.212
N158 G1 X-2.1371
N160 G2 X-2.0396 Y1.2877 R1.212
N162 G1 X.003
N164 G3 X-.1437 Y1.4742 R1.2119
N166 G1 X-1.8929
N168 G2 X-1.6643 Y1.6606 R1.212
N170 G1 X-.3723
N172 G3 X-1.0027 Y1.8471 R1.2119
N174 G1 X-1.0339
N176 Z.1 F6.42
N178 G0 Z.25
N180 X.2037 Y.6352
N182 Z.1
N184 G1 Z0.
N186 G3 X-2.2403 R1.222 F24.45
N188 X.2037 R1.222
N190 G1 Z.1 F6.42
N192 G0 Z.25
N194 M5
N196 G91 G28 Z0.
N198 G28 X0. Y0.
N200 M30
%
4xBoy
07-25-2006, 02:41 PM
Man you guys are using surfcam for 3-axis machines?
I still hand write for an 8-axis.
cnc editor is my 2k program for file transfer.
Westy
07-25-2006, 03:13 PM
i'l study up what you guys said about wcs tehn i'll bring more problems to you.
here is what i am playing with gcode wise.:
%
O0000(MACHINE_GROUP_1)
(DATE=DD-MM-YY - 25-07-06 TIME=HH:MM - 14:36)
(MCX FILE -)
(NC FILE - C:\PROGRAM FILES\MASTERCAMX\MILL\NC\MACHINE_GROUP_1.NC)
(MATERIAL - NONE)
( T1 | 1/2 FLAT ENDMILL | H1 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
/ N104 G91 G28 Z0.
/ N106 G28 X0. Y0.
/ N108 G92 X10. Y10. Z10.
N110 T1 M6
N112 G0 G90 X-1.0339 Y-.5767 S3056 M3
N114 G43 H1 Z.25
N116 Z.1
N118 G1 Z0. F6.42
N120 X-1.0027 F24.45
N122 G3 X-.3723 Y-.3903 R1.212
N124 G1 X-1.6643
N126 G2 X-1.8929 Y-.2038 R1.212
N128 G1 X-.1437
N130 G3 X.003 Y-.0174 R1.212
N132 G1 X-2.0396
N134 G2 X-2.1371 Y.1691 R1.212
N136 G1 X.1005
N138 G3 X.161 Y.3555 R1.212
N140 G1 X-2.1976
N142 G2 X-2.2267 Y.542 R1.212
N144 G1 X.1901
N146 G3 X.1937 Y.6352 R1.212
N148 X.1901 Y.7284 R1.212
N150 G1 X-2.2267
N152 G2 X-2.1976 Y.9148 R1.212
N154 G1 X.161
N156 G3 X.1005 Y1.1013 R1.212
N158 G1 X-2.1371
N160 G2 X-2.0396 Y1.2877 R1.212
N162 G1 X.003
N164 G3 X-.1437 Y1.4742 R1.2119
N166 G1 X-1.8929
N168 G2 X-1.6643 Y1.6606 R1.212
N170 G1 X-.3723
N172 G3 X-1.0027 Y1.8471 R1.2119
N174 G1 X-1.0339
N176 Z.1 F6.42
N178 G0 Z.25
N180 X.2037 Y.6352
N182 Z.1
N184 G1 Z0.
N186 G3 X-2.2403 R1.222 F24.45
N188 X.2037 R1.222
N190 G1 Z.1 F6.42
N192 G0 Z.25
N194 M5
N196 G91 G28 Z0.
N198 G28 X0. Y0.
N200 M30
%
Fancy part you got going there.
Man you guys are using surfcam for 3-axis machines?
I still hand write for an 8-axis.
cnc editor is my 2k program for file transfer.
A screw machine perhaps? Makes sense for that but hand written code isn't practical for simultaneous 3 axis sculpting. ~.5 million lines of code takes a while to type.
Fancy part you got going there.
cool washer mold huh.
i just wanted somthing easy to start.
it goes to line 108 then i get a 09 error.
unusable character was input in significant area.
what in the next line
N110 T1 M6
Westy
07-25-2006, 05:06 PM
If I remember from the pictures you posted there was no tool changer on your machine. If that is the case the T1 M6 will cause a problem as the control will not know what to do with the code. The H1 code calls the tool diameter offset for that tool, you just need to use the D and H codes to keep track of your tool offsets.
buildyourown
07-25-2006, 07:46 PM
Hey Alex,
You've got a lot of questions. I'll work backwards.
The error you got on line 108 is because you don't have a tool changer. M6 is auto tool change. You need to edit your post to substitute a "G91 G28 Z0; M0;
This will bring the spindle up and stop so you can manually change the tool.
More on the "post" This is the intermediary program that converts the mastercam file to a useable .txt file. It doesn't matter what cam you are using, you need a post. Mastercam is one of the better systems because it has a post for almost every machine ever made. I made just a few lines of hand edits to get mine working perfectly with my 24 yo machine.
Does your machine have "multiply work offsets"?
I noticed your program never called a work offset so it will default to G53. Press the offset button on your control. Then press the "work" soft key. This may be slightly off but it's very common.
If there is only 1 offset, you need to "set" x0y0. If you have multiply offsets, you need to set x0y0 and make sure that your program is referencing the correct offset (ie, g54, g55, etc.)
PM me if you have more questions. If you let me know the exact model of control, I can be more specific.
I can also help you with Mastercam and your required posts.
buildyourown
07-25-2006, 07:47 PM
The H1 code calls the tool diameter offset for that tool, you just need to use the D and H codes to keep track of your tool offsets.
H calls the tool length offset, D calls the cutter comp offset.
Westy
07-25-2006, 10:29 PM
H calls the tool length offset, D calls the cutter comp offset.
CraSH!
Whoops. I rarely make parts on machines but spend mind numbing hours making machines.
4xBoy
07-29-2006, 12:19 PM
A screw machine perhaps? Makes sense for that but hand written code isn't practical for simultaneous 3 axis sculpting. ~.5 million lines of code takes a while to type.
Screw Machine, how quaint a name.
Swiss Lathe thank you.
Sorry titles seem to mean everything these days.
But yes I run 7 axis and a 8 axis swiss, not really interested is 3-axis mills and most people don't like turning so my focus has always been lathes.
vBulletin® v3.7.1, Copyright ©2000-2008, Jelsoft Enterprises Ltd.