Mach3 CNC Router Parts 4x2 Router?

Mach3 CNC Router Parts 4x2 Router?

Postby dbrook » Wed Jul 31, 2019 3:40 am

An older gentlemen located near me has purchased a 4x2 CNC Router Parts kit and it is working fine. When he clicks on the REF ALL HOME button the machine homes as normal to the front left corner with the spindle raised to the top limit. When he then checks machine coordinates the DRO’s show X 0.000, Y 0.000 and Z 8.000.

Does anybody have any idea what is causing the DRO for the Z axis to read 8.000 instead of the typical 0.000? Maybe this is normal for a cnc router parts machine but when the following VB script is run the spindle does not move down to the 4” position but slams to the upper most travel position hitting the top limit.

CODE “G53 G00 Z4”

I have searched for a cnc router parts forum for answers but apparently one does not exist.

Any assistance will be most appreciated.

Dan
dbrook
Vectric Apprentice
 
Posts: 64
Joined: Wed Jul 27, 2011 3:36 am
Location: Starkville, MS
Model of CNC Machine: 4x4 DIY Router

Re: Mach3 CNC Router Parts 4x2 Router?

Postby Adrian » Wed Jul 31, 2019 8:11 am

If the machine is at the top of the travel on the I would expect it to read 8" or similar,0 should be near the bottom of the travel. If you were expecting the Z to move down by 4" the Z move should be negative otherwise it's doing what I would expect. Move up 4" from the current position but it can't do that as there's no more room in the Z+ direction.
User avatar
Adrian
Vectric Archimage
 
Posts: 9597
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Mach3 CNC Router Parts 4x2 Router?

Postby Adrian » Wed Jul 31, 2019 8:49 am

Thinking about it the 4" move should be absolute not relative (at least on machines I've owned). When you say it goes to the top limit is it trying to move past that? If so the readout and movements would be wrong from that point as it would have lost steps unless it's a limit switch rather than a physical stop. The home Z position (again on my machines) is always just below the top limit not 0 otherwise moving to home would plough through clamps and all sorts.
User avatar
Adrian
Vectric Archimage
 
Posts: 9597
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Mach3 CNC Router Parts 4x2 Router?

Postby ger21 » Wed Jul 31, 2019 11:53 am

Config > Homing / Limits > Home Offset.
He probably has 8 for the Z offset.
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1481
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Mach3 CNC Router Parts 4x2 Router?

Postby dbrook » Wed Jul 31, 2019 2:36 pm

Thank you Adrian and ger21 for the prompt reply. When I checked the soft limits on Z there was a value of 8.000 set in the Z offset column. When I changed the Z offset to 0.000 the DRO’s showed x 0.000., y 0.000 and z 0.000.

It seems to me that when the VB script was run the spindle should move down to the 4” position. I guess I am thinking about it wrong.

Please tell me why you would want the 8.000 offset in in the Z soft limit?
dbrook
Vectric Apprentice
 
Posts: 64
Joined: Wed Jul 27, 2011 3:36 am
Location: Starkville, MS
Model of CNC Machine: 4x4 DIY Router

Re: Mach3 CNC Router Parts 4x2 Router?

Postby IslaWW » Wed Jul 31, 2019 2:58 pm

"It seems to me that when the VB script was run the spindle should move down to the 4” position. I guess I am thinking about it wrong."

Yes you are. With the machine Z zero position at the top of its travel (desired) you would need to enter "G53 Z-4" to move down 4 inches. Remember machine coordinates (G53 coords) are top down. User or work coordinates are bottom up
Gary Campbell
CNC Technology & Training
The Ultimate Woodworking Machine
GCnC411 (at) gmail.com
User avatar
IslaWW
Vectric Wizard
 
Posts: 1264
Joined: Wed Nov 21, 2007 11:42 pm
Location: Marquette, MI, USA
Model of CNC Machine: The Ultimate Woodworking Machine

Re: Mach3 CNC Router Parts 4x2 Router?

Postby TReischl » Wed Jul 31, 2019 2:59 pm

dbrook wrote:Thank you Adrian and ger21 for the prompt reply. When I checked the soft limits on Z there was a value of 8.000 set in the Z offset column. When I changed the Z offset to 0.000 the DRO’s showed x 0.000., y 0.000 and z 0.000.

It seems to me that when the VB script was run the spindle should move down to the 4” position. I guess I am thinking about it wrong.

Please tell me why you would want the 8.000 offset in in the Z soft limit?

On that machine you don't want anything but 0 in that offset.



The thing to remember about homing a machine is that it tells the machine where it is space. Those are machine zeroes, not part program zeroes. You do NOT want to attempt to run any program with the machine zeroes as your part program zero.

Edit: As Isla mentioned, G53 is a special case, you should not be using it for programming parts. Your mach3 post processor automatically puts a G54 in the beginning of the program to prevent the G53 from being the workpiece coordinate system.

There are a slew of "offsets" aka "workpiece coordinates" that are used to tell a machine where part program zero is located in reference to the machine home/origin. Most of the time on that machine (mine is a CNC RP type machine with Mach 3 also) the program will contain the command "G54" at the beginning. That command references the workpiece offset that has been set in X,Y,Z axis. When you move the axis to the zero point on your workpiece and press the X,Y,Z zero buttons what happens is those values are stored in the G54 offset registers. From then on the machine control does the math between the G53 registers (machine origin) and the G54 registers to position the machine while the part program is running.

Why so "complicated"? Because it is handy to be able to program multiple fixtures (locations) on the table with each one having its own zero points. Quite often I have two vises on my machine. Both of them use the rear jaw and the right end of that jaw as zero. So when I program I can just program each part individually and not worry about the relationship to the other part. I set G55 for one and G56 for the other one. Those are also workpiece registers.

So what I am getting at here is that after you home the machine, then you need to move to zero positions and set them. So if you set Z zero at the top of the workpiece when you command Z4.00 the Z axis will move 4 inches above the surface of the workpiece.

It sounds to me like someone was trying to program the machine from machine origins and figured that since the axis could move 8 inches that was a good number to use. The problem with that is each tool sticks out of the spindle a different amount. In other words, trying to program from machine zero does not work.
"If you see a good fight, get in it." Dr. Vernon Jones
User avatar
TReischl
Vectric Wizard
 
Posts: 2864
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Mach3 CNC Router Parts 4x2 Router?

Postby ger21 » Wed Jul 31, 2019 3:06 pm

Maybe this is normal for a cnc router parts machine but when the following VB script is run the spindle does not move down to the 4” position but slams to the upper most travel position hitting the top limit.

CODE “G53 G00 Z4”



Are you sure the Z axis is not moving backwards?


(I need to start reading the entire posts before replying....)
Gerry - http://www.thecncwoodworker.com
ger21
Vectric Wizard
 
Posts: 1481
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Mach3 CNC Router Parts 4x2 Router?

Postby dbrook » Wed Jul 31, 2019 9:44 pm

Thanks for all the excellent feedback. Your responses have cleared it up for me.

Dan
dbrook
Vectric Apprentice
 
Posts: 64
Joined: Wed Jul 27, 2011 3:36 am
Location: Starkville, MS
Model of CNC Machine: 4x4 DIY Router


Return to Control Software related questions

Who is online

Users browsing this forum: Jim_Nestor and 1 guest