Z axis gets off

[ger21]

Do you have any M codes in your Initialization string in General Config? Or custom M codes in your g-code?

[RCaffin]

Hi Gerry

If there was something in the init string, wouldn't that show up on the DRO?

Cheers
Roger

[ger21]

Typically, yes, but it could also be changing the DRO.
I don't really understand how what he's seeing could be happening.

[RJ02]

Not sure about the initilization and any M codes in Mach3, but I did notice that when I first start Mach3 and load a file, and I had to slow the velocity way down to notice this. I zero the Z and when I click cycle start, the Z DRO goes from zero to -1.00, then starts climbing to .25 and the actual Z is going up 1.25 and DRO reads .25. Sorry for the delay, but at work. Thanks you guys!

[ger21]

Sounds like you have a G43 tool length compensation that is applied in the g-code. When you zero the second time, it's still in effect, so your Z zero is correct the second time.

[RCaffin]

Sounds like you have a G43 tool length compensation that is applied in the g-code.

I think Gerry has got it.
Zero the tool table and Save Settings.

Cheers

[RJ02]

Well I tested your diagnoses and it is the G43 causing the problem. If I take it out of the code, the problem goes away. I don't think I need it anyway, so I'll have to change tool length offset to 0 when selecting tool in Dolphin cam. It puts G43 in automatically. At least I couldn't find where to tell it not to.
As for the save settings after zeroing, I tried that and it worked on some G code files but not on all, so I think my best bet is to change tool length offset to zero in cam, or remember to delete it from the code before using it.
Thanks guys for all your help! I really appreciate it. I would have never figured this out on my own.

Robert

[RCaffin]

Our invoice is in the mail ...
:-) :-)

Cheers
Rogr

[bhurts]

Just my opinion but your better off zeroing the tool and leaving the actual z offset alone. Just list all your tools as tool one in cam and then when you change tools zero your tool 1 offset instead of z.

Ben

[RJ02]

Not sure I understand what you mean by zeroing tool 1 offset instead of Z. Could you explain procedure?
Thanks

[bhurts]

Jog the tool to where you want zero to be like normal. Then pic the offsets tab at the top of your screen. On the bottom right is the tool information box. Leave the gauge block height at zero. Click beside where it says tool and change the number to 1 and press enter. Then click the set tool offset button. Then go to save tool offsets. It should bring up the tool table window. Tool 1 should have a negative z value that is your z zero point in the height column. If that looks good hit apply and ok. Now go to the mdi screen and type in G49 and hit enter. This should change the z value to wherever you are at right now in relation to true machine zero. Now type in G43 H1 and hit enter. That should change the z readout to where you are in relation to how you zeroed your tool. I hope this also shows you why the cam program adds these codes to your code. As a disclaimer I do not use mach 3 myself. I used it briefly years ago and had to open up an old copy to make this reply. Someone who uses the program may take a different approach.

Ben

[RCaffin]

> Could you explain procedure?
Offsets (Alt 5)
Click on Save Tool Offsets bottom RH corner
Zero all entries.
Apply, OK, Config/Save Settings

Having unknown stuff in the Tool Table can be ... dangerous! Zero is always safe.

Cheers
Roger

[skware]

I am having exact same problem I get the machine zeroed with DRO it works once then the next time I try the machine has re-set its soft limits/machine coordinates by roughly 1/2 inch or hovers above a job even if it's been zeroed to the face of the material it's supposed to be cutting? If you figure out what's wrong with yours please let me know. Cheers amos


Sent from my iPhone using Tapatalk

[RJ02]

Thanks, I'll give it a try tonight.