[ballistic42]

Having a problem with the Z soft limit warning in mach3. My mill is a G0704 CNC conversion. I have the X,Y and Z all zeroed out on the DRO for the part I am going to cut. Everything looks good then go to load the program and proceed to hit cycle start and the machine moves to a location for the tool change. I put the tool in then it moves to the safe Z location the spindle starts and then it starts going up and hits the soft limit switch on the Z axis. Here is the Gcode that is giving me problems. My Z soft limits are set at .30 and the safe Z limit is set at -.50 Machine Cordinate. Any help would would be awesome.

Jeff

( Made using CamBam - CamBam CNC Software )

( M1 AR15 side pins 3/12/2015 1:44:53 PM )

( T4 : 0.375 )
( T14 : 0.156 )
( T15 : 0.376 )
( T16 : 0.125 )

( STOCK/BLOCK,7.6875,1.304,1.0,0.0,1.304,1.0 )

G20 G90 G91.1 G64 G40

G0 x-4.0 Y0 Z0.5

( T4 : 0.375 )

( TOOL/MILL,0.375,0.0,4.3051,0 )

T4 M6 G43 H4

( Drill1 )

G17

M3 S2300

G0 X1.931 Y-0.714

G98

G0X1.931Y-0.714Z0.25

G83 X1.931 Y-0.714 Z-1.0 Q0.25 R0.25 F10.0

G0 x-4.0 Y0 Z0.5

G80

( Drill2 )

G0 X-4.0 Y0 Z0.5
( T15 : 0.376 )

( TOOL/MILL,0.376,0.0,5.6406,0 )

T15 M6 G43 H15

M3 S2300

G98

G0X1.931Y-0.714Z0.25

G81 X1.931 Y-0.714 Z-1.0 Q0.25 R0.25 F5.0

G0 X-4 Y0 Z0.5

G80

( Drill3 )

G0 x-4.0 Y0 Z0.5

( T16 : 0.125 )

( TOOL/MILL,0.125,0.0,4.11290,0 )

T16 M6 G43 H16

M3 S2300

G0 X3.899 Y-0.625

G98

G0X3.899Y-0.625Z0.25

G83 X3.899 Y-0.625 Z-1.0 Q0.25 R0.25 F5.0

G0 Z0.5

G0X3.056Y-0.939Z0.25
G83 X3.056 Y-0.939 Z-1.0 Q0.25 R0.25 F5.0

G0 X-4 Y0 Z0.5

G80

( Drill4 )

G0 X-4.0 Y0 Z0.5

( T14 : 0.156 )

( TOOL/MILL,0.156,0.0,4.5707,0 )

T14 M6 G43 H14

M3 S2300

G0 X3.899 Y-0.625

G98

G81 X3.899 Y-0.625 Z-1.0 R0.125 F5.0

G81 X3.056 Y-0.939 Z-1.0

G80

G0 X-4 Y0 Z.5

M5

M30

[mactec54]

ballistic42

You can't have the Soft limit set behind the Limit Switch, must be the same setting as the limit, or just below the limit, your program format is a mess I don't know why Cam Bam have not fixed their post processors to output a better program format, what is programed is a crash waiting to happen

[ger21]

Do you have a Z home switch? And are you homing the Z when you start the machine?
The Z softlimits are relative to the home position,so if you're not homing, they could be lower than they should be.
Also, are your tool length offset correct? Do you have the right length in the tool table?

[ballistic42]

Mactec54, Here are my settings for home and limit switches.

AXIS SOFT MAX SOFT MIN SLOW ZONE
Z 0.00 -8.15 .30
X 17.3 0.00 .50
Y 3.25 0.00 .50
I know this much it works when slowing to the limit switches in either direction. I have one switch for each axis. i home to the negative side of the axis if that helps. Again I made my safe Z for the Z axis 0 now, but still get the same results. The Z axis works fine up until the table returns from X-4 Y0 Z.5. The Z starts to go up and hits the limit switch. I do not know why this is happening.

Jeff

[ballistic42]

Gerry, Sorry did not see your post. Yes I am homing the Z and yes i do have a limit switch on the Z axis. I am running one switch per axis for home and soft limits. I have bolts at the max Z and the min Z to trip the axis when it reaches its limit. It works fine for all three axis. I start the machine and home it (all axis home to the negative position) then with my part in the vise I jog to the upper right corner of the part and zero each axis out. I am using the Haimer ZERO MASTER for this(very accurate.) I have all my tooling in the TTS holders and have all the heights for each tool in the tool table using the Tormach Tool Assistant. I have the Haimer in its own TTS holder and used the Tormach Tool Assistant to measure the height of the Haimer with it indicating zero and that is my tool 50 in my mach3 tool table.

I just cannot figure out why the Z axis tries to go up to the top after the tool change (Manual tool change by the way.) The Gcode I put in was a G0 X-4 Y0 Z.5 for the tool change location, this was to get the part out from under the spindle so i could change the tool. When the tool is put in I hit cycle start again and the X and Y move to the right spot but the Z starts going up to the Z max and hits the limit switch. While this is going on the spindle just sits and spins at the selected RPM of 2300 which is correct via Gcode, but the program just stops and says that the Z limit was reached. I understand that the Z limit is reached because I can see the Z axis is moving all the way to the top and of course is hitting ther limit switch. Why it goes up like that is the million dollar question. No where in the coding do I see where I have told it to do that.


Jeff

Jeff

[ballistic42]

Gerry, sorry my mistake I jog to the upper left corner of my part(need more coffee).

[ger21]

My guess is that it's your tool length offset.

[mactec54]

ballistic42

As Gerry has said it most likely is you tool offsets, once you have homed your machine, then the soft limits can be set anywhere below or in front of the limit switches, can not be set behind a limit switch, are you setting each tool to the top of your part, or are you trying to do some other tool setups

Never do a Z move with a X & Y move, you should always move the Z axes up first, then move the X & Y

A G80 should be directly after each canned cycle
A G98 or G99 should be used in the same line as the canned cycle, a G98 will retract to the Z axes value, .5 in your case, If using a G99 this will retract the Z axes to the R value that is used in the canned cycle




%
G17G20 G90 G91.1 G64 G40
G0Z.5
G0 x-4.0 Y0
T4 M6 ( T4 : 0.375 )
G54
M3S2300
G43Z.5 H4
G90G0 X1.931 Y-0.714
G0Z.250
G83G98 X1.931 Y-0.714 Z-1.0 Q0.25 R0.25 F10.0
G80G0Z.5
G0 x-4.0 Y0.




T14M6 ( T14 : 0.156 )
G54
M3 S2300
G43Z.5 H14
G90G0 X3.899 Y-0.625
G81G98 X3.899 Y-0.625 Z-1.0 R0.125 F5.0
G80G0Z.5
G0 X-4 Y0
M5
M30
%

[ballistic42]

Gerry, I think you are right. i have the right tool length set right. What I was doing wrong was in the offsets page of mach3, the Tool Offset ON/OFF was either on or off not sure what the LED is telling me. All I know is a zeroed out the Z axis with the Haimer and then toggled zero on the Z axis then clicked on the LED toggle in offsets and the axis was zeroed. I redid the Cam Gcode and ran the part (WAX block to start with). The machine ran GREAT no problems. I think a few things were going #1 The Gcode was wrong and the code was written for mach3/cutviewer. #2 I was not sure how the Offsets page Tool Offset ON/OFF worked. As I played and made some mistakes, I have figured it out so far. All I can is Thank Goodness for the pendant with that BIG RED BUTTON!!! The E-stop has saved my mill from crashing bigtime several times!!! The Haimer Zero Master was not cheap so I am taking great care in how I proceed from here on out.

All that being said, one problem that I am running into is when the Mill goes to the .20 up from the work piece for the manual tool change in mach3 M6. The tool is right over the work part. I put a G0 X-4 y0 right after the G0 Z.20. this way the Z axis will go up Z .20 then go over G0 X-4 Y0. At that position I can change the tool. Is there a way in the M6 macro to program this and if so how would I do that. A little background I have only been doing this coding for a few days now. I bought the G0704 Mill 6 months ago and have just got to this point. I have been reading like crazy but hard to learn this much stuff in a short amount of time on my own.

Thanks,

Jeff

[ballistic42]

Here is the new Gcode from CamBam for mach3. What I dont understand everyone talks about G43 H(index number). My coding does not have that so why not and why does it work?
( Made using CamBam - CamBam CNC Software )

( M1 AR15 side pins 3/14/2015 12:27:58 PM )

( T4 : 0.375 )

( T14 : 0.156 )

( T15 : 0.376 )

( T16 : 0.125 )

G20 G90 G91.1 G64 G40

G0 Z0.2
G0 X-4 Y0

( T4 : 0.375 )

T4 M6
( Drill1 )

G17

M3 S2300

G0 X1.931 Y-0.714

G98

G83 X1.931 Y-0.714 Z-0.904 Q0.25 R0.2 F5.0

G80
( Drill2 )

G0 Z0.2

( T15 : 0.376 )

T15 M6

M3 S2300

G98

G81 X1.931 Y-0.714 Z-0.904 R0.0 F5.0

G80

( Drill3 )

G0 Z0.2

( T16 : 0.125 )

T16 M6

M3 S2300

G0 X3.056 Y-0.939
G98

G83 X3.056 Y-0.939 Z-0.904 Q0.25 R0.2 F5.0

G83 X3.899 Y-0.625 Z-0.904

G80

( Drill4 )

G0 Z0.2

( T14 : 0.156 )

T14 M6

M3 S2300

G98

G81 X3.899 Y-0.625 Z-0.904 R0.0 F5.0

G81 X3.056 Y-0.939 Z-0.904

G80

G0 Z0.2

M5

M30

[ballistic42]

mactec54, thanks for the help in the coding. I have spent the last 3 days trying to figure what all this code means. I think I have a much better understanding of it. I finally got the code done tonight and ran the wax block twice with no problems. I was watching a Tormach video and I put a G28 for my tool change, it works great. My mill is the G0704 so the table is small so going to home for the G28 is not a big deal to me. Would be cool to figure out how to set a G28 with different X,Y, and Z coordinates so that it would not goto the machine coordinates each time.

I had to turn off the safe Z because it kept tripping my switch for some reason. With the safe Z turned off and the soft limit switch on the program ran fine. Not sure why the Safe Z was throwing me such a fit. Here is what the final code came out to be.

Thanks again guys for all the help!!
Jeff
( Made using CamBam - CamBam CNC Software )

( M1 AR15 side pins 3/14/2015 12:27:58 PM )

( T4 : 0.375 )

( T14 : 0.156 )

( T15 : 0.376 )

( T16 : 0.125 )

G20 G90 G91.1 G64 G40

G28

( T4 : 0.375 )

T4 M6 G43 H4

( Drill1 )

G17

M3 S2300

G0 X1.931 Y-0.714

G83G98 X1.931 Y-0.714 Z-0.904 Q0.25 R0.2 F5.0

G80

( Drill2 )

G28

( T15 : 0.376 )

T15 M6 G43 H15

M3 S2300

G81G98 X1.931 Y-0.714 Z-0.904 R0.0 F5.0

G80

( Drill3 )

G28

( T16 : 0.125 )

T16 M6 G43 H16

M3 S2300
G0 X3.056 Y-0.939

G83G98 X3.056 Y-0.939 Z-0.904 Q0.25 R0.2 F5.0

G83 X3.899 Y-0.625 Z-0.904

G80

( Drill4 )

G28

( T14 : 0.156 )

T14 M6 G43 H14

M3 S2300

G81G98 X3.899 Y-0.625 Z-0.904 R0.0 F5.0

G81 X3.056 Y-0.939 Z-0.904

G80

G28

M5

M30