Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: spr203 on June 25, 2012, 08:51:00 PM
-
hi, i am having a problem and i am sure it is me not the machine . here is whats going on i use cambam to write my programs and i am running a part i need to drill 5 different hole sizes. and mill a slot . the program will not use the tool offsets . i know i must be missing something . any help Will be great . thanks guys
-
Do you have the tool table set up for your tools? How is your CAM calling the tools? Is your CAM producing a true tool path based on the tool Dia or is it expecting Mach to do the dia offset?
Hood
-
Hi spr203 are you using a drawing and setting the parameters in the TOOL section at the bottom of Cambam's MOP. if so cambam should set tool paths. Post you cambam file here or in CAMBAM forum and I'll take a look
-
hi here is my program i am using .
( 4in Roller Post Spider Crossmember 6/25/2012 3:00:24 PM )
( T5 : 0.5 )
( T6 : 0.78 )
( T7 : 0.81 )
( T19 : 0.5 )
( CUTVIEWER )
( FROM/0,0,5 )
( Select dummy tool to avoid warnings )
( TOOL/MILL,1,0,20.0,0 )
( STOCK/BLOCK,,,,,, )
G20 G90 G91.1 G64 G40 g43
G0 Z0.125
( T5 : 0.5 )
( Tool Taper coming soon )
( TOOL/MILL,0.5,0.0,0.0,0 )
T5 M6
( Drill1 )
G17
M3 S1000
G0 X15.0376 Y9.3985
G98
G81 X15.0376 Y9.3985 Z-0.7 R0.125 F10.0
G81 X10.2757 Z-0.7
G81 X5.7644 Z-0.7
G81 X1.0025 Z-0.7
G81 X2.005 Y7.4767 Z-0.7
G81 Y4.7619 Z-0.7
G81 Y2.0471 Z-0.7
G81 X4.01 Y4.7619 Z-0.7
G81 X12.0301 Z-0.7
G81 X14.0351 Y2.0471 Z-0.7
G81 Y4.7619 Z-0.7
G81 Y7.4767 Z-0.7
G80
( Drill2 )
( T6 : 0.78 )
( Tool Taper coming soon )
( TOOL/MILL,0.78,0.0,0.0,0 )
T6 M6
M3 S1000
G0 X2.005
G98
G81 X2.005 Y7.4767 Z-0.7 R0.125
G81 Y2.0471 Z-0.7
G81 X14.0351 Z-0.7
G81 Y7.4767 Z-0.7
G80
( Drill4 )
G0 Z0.25
( T7 : 0.81 )
( Tool Taper coming soon )
( TOOL/MILL,0.81,0.0,0.0,0 )
T7 M6
M3 S1000
G0 Y4.7619
G98
G81 X14.0351 Y4.7619 Z-0.8 R0.25
G81 X12.0301 Z-0.8
G81 X4.01 Z-0.8
G81 X2.005 Z-0.8
G80
( Profile1 )
( T19 : 0.5 )
( Tool Taper coming soon )
( TOOL/MILL,0.5,0.0,0.0,0 )
T19 M6
M3 S1000
G0 X3.4375 Y9.3226
G1 Z-0.125
G1 F8.0 X0.3
G1 Y9.4744
G1 X15.7401
G1 Y9.3226
G1 X3.4375
G1 F10.0 Y9.2726
G1 F8.0 X0.25
G1 Y9.5244
G1 X15.7901
G1 Y9.2726
G1 X3.4375
G1 F10.0 Y9.3226
G1 Z-0.25
G1 F8.0 X0.3
G1 Y9.4744
G1 X15.7401
G1 Y9.3226
G1 X3.4375
G1 F10.0 Y9.2726
G1 F8.0 X0.25
G1 Y9.5244
G1 X15.7901
G1 Y9.2726
G1 X3.4375
G0 Z0.25
M5
M30
-
You have no G43 H(whatever tool number) on the M6 line. Should look like this:
T5M6G43H5 for your first drill
-
and also... you don't have the tools rapiding to a safe Z position, you are looking for a crash....
should look like this:
T5M6G43H5
G0Z.1
Then proceed with the drilling or milling.
-
thanks guys . i got it working about 75% i would say . i have about 4" difference in length of tools . when i but my 3rd tool in it drills the hole to correct depth but it retrats almost to z home . i know i'm missing something there also .
-
G49 Z0
That will cancel the tool length offset and retract the machine to Z0 of the machine, on a mill, that's usually all the way up, or retracted on the quill.
-
i must not be doing something correct . here is how my program looks now . when i go to tool number 7 it drill hole fine but after drilling moves up away from part 3" . this isn't the end of the world just looking to cut time . also is there any better way to mill a slot other than the way i have it cutting now ? thanks
( STOCK/BLOCK,,,,,, )
G20 G90 G91.1 G64 G40
g0z.125
( T5 : 0.5 )
( Tool Taper coming soon )
( TOOL/MILL,0.5,0.0,0.0,0 )
T5 M6
( Drill1 )
G17
g43 h 5 m8
M3 S1000
G0 X15.0376 Y9.3985
G98
G81 X15.0376 Y9.3985 Z-0.7 R0.125 F3.5
G81 X10.2757 Z-0.7
G81 X5.7644 Z-0.7
G81 X1.0025 Z-0.7
G81 X2.005 Y7.4767 Z-0.7
G81 Y4.7619 Z-0.7
G81 Y2.0471 Z-0.7
G81 X4.01 Y4.7619 Z-0.7
G81 X12.0301 Z-0.7
G81 X14.0351 Y2.0471 Z-0.7
G81 Y4.7619 Z-0.7
G81 Y7.4767 Z-0.7
G80
g0 z.25 x-.5 y 2.5 m9
( Drill2 )
G0 Z0.125
( T6 : 0.78 )
( Tool Taper coming soon )
( TOOL/MILL,0.78,0.0,0.0,0 )
T6 M6
g43h6m8
M3 S1000
G0 X2.005 Y7.4767
G98
G81 X2.005 Y7.4767 Z-0.8 R0.125
G81 Y2.0471 Z-0.8
G81 X14.0351 Z-0.8
G81 Y7.4767 Z-0.8
G80
g0z.25x-.6y2.5m9
( Drill4 )
( T7 : 0.81 )
( Tool Taper coming soon )
( TOOL/MILL,0.81,0.0,0.0,0 )
T7 M6
G43h7m8
M3 S1000
G0 X14.0351 Y4.7619
G98
G81 X14.0351 Y4.7619 Z-0.8 R0.25
G81 X12.0301 Z-0.8
G81 X4.01 Z-0.8
G81 X2.005 Z-0.8
G80
g0z.25x-.6y2.5
( Pocket1 )
( T20 : 0.75 )
( Tool Taper coming soon )
( TOOL/MILL,0.75,0.0,0.0,0 )
T20 M6
g43h20m8
M3 S1000
G0 X-0.425 Y9.3976
G1 Z-0.07
G1 F4.0 Y9.3994
G1 X16.625
G1 Y9.3976
G1 X-0.425
( pocket2 )
M8
S1000
G0 Z0.25
G0 X16.625
G1 F10.0 Z-0.14
G1 F3.0 X-0.425
G1 Y9.3994
G1 X16.625
G1 Y9.3976
( Pocket3 )
m8
S1000
G0 Z0.125
G0 X-0.443 Y9.3796
G1 F10.0 Z-0.25
G1 F3.0 Y9.4174
G1 X16.643
G1 Y9.3796
G1 X-0.443
g0z.25x-.6y2.5m9
G0 Z0.125
M5
M30
-
I copied the code over into G-Wizard editor and ran it, I don't see anything moving higher than .25 above the part. What sort of machine is this, how do you do tool changes without coming up in the air at some point? Where are you getting this code? I've never seen something put Z values before XY values.... that's usually not good form.... it's always XYZ in that order. Also, on your G81 lines, after the first line where you define everything, all you need is the next X or Y position, no Z value necessary.... unless I suppose you wanted to change depth.
-
hi was again thanks for the help.
i use cambam to make the program . at this point either camabm is giving me something wrong or i am setting up mach3 tools wrong .
how i set my tools are i put the shortest one in set my zero and then go to tool offsets eneter my tool number in this case 20 and hit the offset button and then save and apply . i go to my next shortest tool number 7 do the samething touch off surface of part then hit the button for tool offset. and so on for the tools .
i use a position outside of the part i have in the machine for my tool chage area.
-
Well, I'm not very good with Mach, my machine is a different software, but I help a friend with Mach, so I have some knowledge. Where your issues are coming from, I can't say, and I know that there are lots of different ways to get the same thing accomplished. My process goes something like this:
Home the machine, that usually is fully X minus, Y minus and Z plus, then go indicate or edge find the part and determine where I wand X0 Y0 to be. In Mach, you then zero the X and Y readout, that enters the part position into G54, leaving the Z alone.
Now, put your first tool, regardless of length, into the quill and bring it down to touch the Z0 level of the part, set that tool dimension to the tool number in your program accordingly. Do the same with the other tools. Double check your tool dimension table and make sure that the values correspond with what you got with the tools touching the Z0 level.
In your program, like I said, your tool call will now be T01 M06 G43 H01, then your first move after you get to your position will be G00 Z.1, that will rapid down to .100" above the part, then proceed with your machining.
After you have drilled/milled, rapid up to Z.1, then your next line will be G49 Z0, this cancels the tool length offset and returns the Z axis to the top. You need to do that after each tool to cancel that tools offset.
Do your tool change, and proceed thru all of your tools in the same fashion. It doesn't matter which tool is longest or shortest, as long as they will all reach the part and depth you are machining to with the available stroke you have of the machine... my Z quill is limited to 5", so I have to be careful to have the tools pretty close to the same length. I don't like to be rapiding along just .1 or even .25" above the part... if you have clamps or screws sticking up, or chips lay on the part, you might run into clamps, or drag chips and make marks on your part, the few split seconds of Z movement up and down are not going to make or break you.
That should get you pretty close...
-
really thanks so much that has shed alot of light on what i am doing .