Post Process Mach3

[Anonymous]

Hey everyone! Very new to CNC and it is a lot of information to take in and I am not sure how to approach so I thought I would ask. After setting up my project and going though the post process I am running into the issue that my bit does not rise of the home point (on the z-axis) to jog to its starting point. Its dragged through some of my stock on a few occasions. Also at the end of a run at whatever cutting depth the bit is at it will return home and tear through whatever is in it path.

I've fixed this with adding a line right after G54 that raises the Zed before i jogs over and at the end before it jogs back. And in typing this i realized that this is  most like due to the table not being level (which I am currently coming up with a solution).

My question though is that is there a way to change that in fusion? Or is it normal for it to jog along 0 Z-axis when you start a job?

Thanks again! My apologies for the long read.

[Tom.Hemans]

Hi @Anonymous,

By default, the Mach3Mill post outputs G28 G91 Z0 to go to the maximum Z position on the machine. However, it sounds like on your machine that Z0 is down on the table.

If you can find out the maximum Z position of the machine, then you can modify the post to move to this position at the start/end of an operation. To do this

• open the post in a text editor (e.g. Notepad++)
• use Ctrl + F to find where "zHome" is defined in the post
• change the value of zHome from 0 to the value of the maximum Z height (see the image zHome.png)

Hope this helps,

Tom

[HughesTooling]

@Tom.Hemans  That's bad advice, seems you need to read up on G28 as well. What will happen if you program G28 G91 Z100. is the machine will move up to 100 then go back to the machine Z0.0, the 100 move is incremental before the G28 is performed moving to the machine zero. See here for info on G28.

Also this problem comes up at least once a week and is down to people not having limit switches and/or not homing their machines. The OP should read up on his control and figure out how to set the G53 offsets to a safe position so G28 can be used.

Also Tom Please don't attach pictures. There's an option Photos on the editor toolbar to embed them, please use this option.

Thanks mark

[Tom.Hemans]

Hi @HughesTooling,

I believe G28 is slightly different for Mach3 than for other CNC controllers.

So, @Anonymous if you check the G28 home Z (parameter 1563) of your machine you can see where the tool is retracting to. You can then change this position to a safe height and won't need to modify the post.

Apologies for the confusion,

Tom

[HughesTooling]

This looks the same as what I said, the tool will make an incremental move of Z100. then go to the machine Z0 (G53 Z0.) 

Mark

[daniel_lyall]

@Tom.Hemans  As a Mach3 user of 3 routers and a lathe what @HughesTooling is correct the post is working as intended, A G28 will move the machine to the Machine Zero/Home position after an intermediate move if one is there.

The OP more than likely is not homing the machine so The G28 is doing something wrong.

@Anonymous If you do not have home switches you can do a home in places with Mach3.

You do this by moving the machine to the front left with the Z-axis at almost its max height above the machine bed, you, of course, can do it where ever you want but always have the Z-axis at a hight it will not hit anything and make sure in ports and pins the home switches are not set if you do not have home switches.

This is really important as time goes on every time the machine loses position if the Machine zero/home position is not set the home position could end up being under the bed of the machine or above the top of the Z-axis, both these will cost you lots to fix what broke.