Strange KmotionCNC behavior

[CNCMAN172]

mmurray70,

As i pondered this issue I am really wondering, why would the CAM use the G43 tool offset? Further I guess I really don't understand this clearly. The offset was 3", meaning the tool was three inches long, longer than the vcarve bit in he collect but you would think the only reason it would need to know the length would be to ensure the tool was high enough not to crash into the material before drilling started. That would seem to indicate it should have been drilling in air well above the table. I know the offset is the issue, but I guess I don't really understand the reason for using a tool offset in a drilling cycle.

Russ




( T2 | 1/4 INCH ENGRAVING TOOL 90 DEGREE X .001 TIP LONG | H2 )
N100 G20 ( inch system )
N102 G0 G17 G40 G49 G80 G90 ( Rapid positioning ON, XY Plane Selection, Cancel cutter diameter compensation, Cancel Tool length offset, cancel motion mode, Absolute)
N104 T2 M6 ( Tool#2, tool change)
N106 G0 G90 G54 X.5 Y1. S6000 M3 ( Rapid, Absolute distance, Work Present 1, XY position (.5,1), Spindle 6000, Spindle CW)
N108 G43 H2 Z.1 ( tool length offset, H2 is not populated in tool table)
N110 G99 G81 Z-.215 R.1 F5. ( R value return canned cycles, drilling canned cycle, Z depth = -.215", return to .1", Feedrate 5 )
N112 Y6.2813

[bhurts]

The three inches has nothing to do with the tool length. It is the distance from z zero (home) to the top of the part. You are thinking of g43 all wrong. What you have been doing for years is fine but your case is not typical so cam programs are doing things you are not. This is the easiest way to look at it.

Pretend there is no z zero button for any of the fixture offsets. You can only set x and y. You still need to set a z zero but instead of using the z zero button you set the tool offset for the tool you are using. This effectively does the same thing as setting the z fixture offsets so it has to remain zero. When you touched off at the top of your part you had yet to run the g-code. You set your z fixture offset by bringing the tool down to the top of your part and zeroing. When you ran the codes T1 and then later G43 H1 you called the tool height H1 for tool 1 T1 and put it into effect G43. That combined with the z fixture zero you already set caused the crash. Your machine thought it needed to go 3 inches lower to get to your part. After you crashed the g-code interpreter had been set for T1 H1 and unless you cancelled those offsets they would stay persistent. So now you bring your new tool down to the part and zero z fixture offset again. When you run the code again no crash because setting the z again after the tool offsets had been read effectively cancelled them.

Two fixes either stop using your z fixture offset and set your tool offset instead or erase the codes T1 M6 and G43 H1 from your code before running it.

Ben

Sent from my HTC6525LVW using Tapatalk

[CNCMAN172]

Ben,

Thank you, I understand now. This is setup like the Fadal we had at work that had the tool table with all the lengths stored in the control memory. We use to set material height and that is all. Now I understand should have learned this long ago on my home machine. No tool changer so I ignored this stufff.

Russ