Hello Guest it is December 15, 2019, 07:47:56 PM

Author Topic: Problem running programs on Mach3  (Read 3287 times)

0 Members and 1 Guest are viewing this topic.

Offline JAC

*
  •  57 57
    • View Profile
Problem running programs on Mach3
« on: October 12, 2016, 01:32:24 PM »
Hi, like the topic say, I have problems running the programs on mach3. hope somebody can help me or give me ideas what Im doing wrong.
Several years ago I was planning to machine aluminum parts (simple parts) on my table top mill so I download the demo version of Mach3 to my XP computer to try it first. I made several sample pieces and it works great but I had some medical and family problems so I couldnt continue to try it, after several years now I like to try it again. The problem was that my old XP computer where I had the program burn out so I had to buy a new one with windows 7, I download the Mach3 demo version again and I think I set up everything ok but when I load my old program to cut a sample part  it just star cutting on the wrong position. I rehome the machine a zero on my part several times but still want to cut on the different place than where it suppose.
When I load the old program  it shows the part on one side of my mill table (upper/right side) even though I zero my piece on the center of the table, it also shows the circle on my aluminum piece on the upper right side. I made a new program to see if that would fix it but the new program is different than my old one and I use the same drawing.
Does any body know if they change something on Mach3/Lacy cam in the past years?

Im cutting a circle on an aluminum piece. 4" X 4.250" and the center of circle is at X 2.00 Y2.250
Let me see if I can post the codes and some pics so people can see what Im talking about.

Thank you

Offline Tweakie.CNC

*
  • *
  •  8,024 8,024
  • Super Kitty
    • View Profile
    • Tweakie.CNC
Re: Problem running programs on Mach3
« Reply #1 on: October 13, 2016, 01:36:53 AM »
Pics and code would be useful.

Tweakie.
Success consists of going from failure to failure without loss of enthusiasm.  Winston Churchill.

Offline JAC

*
  •  57 57
    • View Profile
Re: Problem running programs on Mach3
« Reply #2 on: October 13, 2016, 10:52:44 AM »
After checking all my settings on Mach3 and my Gcodes,  X,Y,Z points a lot of times for couple days, finally last night I found the problem.
I dont know why or when it change, but my programs have G90 for absolute programs, after searching online all the Gcodes I found out that if I use IJK in my program now it has to be G90.1 instead of the G90. My programs worked perfect before with the G90.
I tried last night and it cuts the part where it suppose to and its display on center of table.
One other thing I notice when it was running the program is that on the Mach3 screen spindle section, the spindle tab was blinking I think I saw something on the tutorial video, it should be a setting to stop the tab for been blinking. I look for it, beside that now is working perfect, I try the  other sample parts programs later this month.

Thank you.

Offline ger21

*
  • *
  •  6,291 6,291
    • View Profile
    • The CNC Woodworker
Re: Problem running programs on Mach3
« Reply #3 on: October 13, 2016, 01:43:38 PM »
G90 and G90.1 are two completely different settings. You need to use both, not one or the other.

Typically, most CAM programs output code that uses:
G90 - Absolute Coordinates
G91.1 - Incremental IJ mode


G90.1 is Absolute IJ mode.

Not that these codes need to be on separate lines in your program, or the first one will be ignored.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline JAC

*
  •  57 57
    • View Profile
Re: Problem running programs on Mach3
« Reply #4 on: October 15, 2016, 03:06:15 PM »
Hi, Gerry thank you for your reply. Thats  why I dont know how is was working perfect before (several years ago). This is my old program. Im new to the Gcodes so I dont know if this is written correctly but so far is working for me , I still learning.

Old program.

N1 T1 M06
N2 G90 G00 X0 Y0
N3  S1200 M03
N4 G0 Z.5000 M08
N5  X3.1175  Y2.2500
N6  Z0.1000
N7 G1  Z-.6000  F6.00
N8 G2 I2.0000  J2.2500
N9 G0  Z.2000
N10  X3.1575
N11  Z0.1000
N12 G1  Z-.6000 
N13 G2 I2.0000  J2.2500
N14 G0  Z.2000
N15  X3.1975
N16  Z0.1000
N17 G1  Z-.6000 
N18 G2 I2.0000  J2.2500
N19 G0  Z1.7500 M1
N20  X3.205
N21  Z0.1000
N22 G1  Z-.6000 F10 
N23 G2 I2.0000  J2.2500
N24 G0  Z1.7000 M09
N25  X0.000 Y0.0000 M05
N26 M30

New program.

N1 T1 M06
N2 G90.1 G00 X0 Y0
N3  S1200 M03
N4 G0 Z.5000 M08
N5  X3.1175  Y2.2500
N6  Z0.1000
N7 G1  Z-.6000  F6.00
N8 G2 I2.0000  J2.2500
N9 G0  Z.2000
N10  X3.1575
N11  Z0.1000
N12 G1  Z-.6000 
N13 G2 I2.0000  J2.2500
N14 G0  Z.2000
N15  X3.1975
N16  Z0.1000
N17 G1  Z-.6000 
N18 G2 I2.0000  J2.2500
N19 G0  Z1.7500 M1
N20  X3.205
N21  Z0.1000
N22 G1  Z-.6000 F10 
N23 G2 I2.0000  J2.2500
N24 G0  Z1.7000 M09
N25  X0.000 Y0.0000 M05
N26 M30

As you can see the only difference is at G90 to G90.1 but I told you it work perfect before with the G90 only. Im just making a circle on a piece of aluminum. For what you say I need to have both on my program . Does one have to be first or it make no differen .

G90.1 G0 X0 Y0
G90

OR

G90
G90.1 G0 X0 Y0

Thank you for all you help.