How to line up JTech to home position

Post Reply
dwats8841
Posts: 2
Joined: Fri Mar 26, 2021 2:33 am
Model of CNC Machine: Onefinity Woodworker

How to line up JTech to home position

Post by dwats8841 »

I haven't found an easy way to set "home" for the laser. Is there a fire button somewhere to fire a weaken shot to set home position?

User avatar
gkas
Vectric Wizard
Posts: 1217
Joined: Sun Jan 01, 2017 3:39 am
Model of CNC Machine: Aspire, Axiom AR8 Pro+, Axiom 4.2W Laser
Location: Southern California

Re: How to line up JTech to home position

Post by gkas »

I set my XY=0 as normal with my centering tool https://www.amazon.com/gp/product/B078V ... UTF8&psc=1. Now that my axis for the spindle is set to 0, I know the offset from spindle to laser is +80Y. I move the spindle +80Y, then reset XY=0. The laser is now perfectly set.

If you don't know your laser offset: Move your laser to a convenient spot. Set XY=0. Fire laser manually to make a spot. Move your spindle until it is dead over the spot. Your readout should now display your XY offset.

dwats8841
Posts: 2
Joined: Fri Mar 26, 2021 2:33 am
Model of CNC Machine: Onefinity Woodworker

Re: How to line up JTech to home position

Post by dwats8841 »

Awesome. Thanks

wb9tpg
Vectric Craftsman
Posts: 297
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: How to line up JTech to home position

Post by wb9tpg »

I put the G92 command in my laser post processor and it automatically applies the offset for me. If you know or can measure your offset I can show you how
Gary Mitchell
Kentucky, USA

wb9tpg
Vectric Craftsman
Posts: 297
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: How to line up JTech to home position

Post by wb9tpg »

I thought I'd take a few minutes to write up a some of my Postprocessor tips regarding using a J-Tech laser with Vcarve (or Aspire). I use a Shapeoko which is a GCODE machine.

Tip #1 No Z
I have two post processors I use with my laser. One has Z motion and the other removes the Z. An easier way to make the NO Z postprocessor is to copy the postprocessor and change this like in it to include a scale factor.

VAR Z_HOME_POSITION = [ZH|A|Z|1.3|0.00001]

The last portion of that entry take any Z entry and multplies it by 0.00001 which effectively removes it. Just zero your Z axis so your laser is 1/8" above the work surface and your good to go.

Tip #2 Turn Laser Mode On Automaticall

If you're like me you forget to turn laser mode on/off with the $32 command. So I put it in my post processor to do it automatically. I will say you need CNCjs to make this work and will explain why later. I put the following stuff in my post process (section labels included)

begin HEADER
"$32=1"
"%wait"

begin FOOTER
"M5"
"$32=0"
"%wait"

Obviously the $32=1 turns laser mode on and the $32=0 turns it off. I also altered my non-laser post processors to include a $32=0 in their headers to make sure the laser mode is off for those. Now this only works for CNCjs for a few reasons. (1) Some versions of Carbide Motion don't like the $32 in the gcode. (2) You need the "%wait" directive that CNCjs supports. You need this because the $32 command writes to NVRAM and the controller pauses a second doing it following gcode commands are sent to the controller and lost while the write is going on. The "%wait" in CNCjs command tells CNCjs to wait until the $32 is done before proceeding. Without the "%wait" things screw up or hang. And if you're wondering if a "G4 P1" will work; it won't since it's GCODE processed by the controller.

Tip #3 Quit resetting XY zero for your Laser

I have a spindle mounted laser and the offset between the cut with a v-bit and the laser is off by 0.5mm (I think due to tramming errors). That's pretty small but I wanted 0 error so I developed a technique to reduce it to 0. And this technique will work even is your laser is offset by a large amount (like you're using a magnetic mount).

I was cutting patterns with V-Bits and wanted to mount my laser, zero Z like any other bit change, and proceed to burn a pattern that was registered on the previous cuts. I then stumbled on the G92 set of GRBL commands with allow a temporary offset to be set in place. Here is my Header section of my Laser PostProcessor with the commands included.

1 begin HEADER
2 "(Starting Program and turning Laser Mode On)"
3 "$32=1"
4 "%wait"
5 "T42"
6 "G17"
7 "G21"
8 "G90"
9 "G92.1"
10 "G0[ZH]"
11 "G0[XH][YH]"
12 + Now apply a temporaty 0.5mm offset for my laser alignment
13 "G92 X-0.5Y0.5"

So lines 1 thru 8 are pretty standard (see my tip #2 above for lines 3 & 4). The magic starts happening at line 9 which resets any temporary offset that might still be in place. Line 10 & 11 move to true 0 in case an offset was in place. Line 13 implements a new offset of X and Y values and should be whatever values your laser dot differs from your spindle cut. I carve a simple v-carve + and them laser a + and see how different you are. Then keep tweaking them until they align perfectly. You laser toolpaths will then align perfectly with your cuts. Your values for Line 13 will likely be very different than mine.

One more thing. Put the following lines in your Footer section of your laser toolpaths to turn off the offset. I also put them in the Header section of my non-laser post processors so even if a laser toolpath does not complete the offet is removed before making a cut.

+ Reset any offsets in place
"G92.1"

Well that's it for now. These are somewhat advanced concepts and may take you some time to play with and hopefully improve them
Gary Mitchell
Kentucky, USA

wb9tpg
Vectric Craftsman
Posts: 297
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: How to line up JTech to home position

Post by wb9tpg »

I thought I'd take a few minutes to write up a some of my Postprocessor tips regarding using a J-Tech laser with Vcarve (or Aspire). I use a Shapeoko which is a GCODE machine.

Tip #1 No Z
I have two post processors I use with my laser. One has Z motion and the other removes the Z. An easier way to make the NO Z postprocessor is to copy the postprocessor and change this like in it to include a scale factor.

VAR Z_HOME_POSITION = [ZH|A|Z|1.3|0.00001]

The last portion of that entry take any Z entry and multplies it by 0.00001 which effectively removes it. Just zero your Z axis so your laser is 1/8" above the work surface and your good to go.

Tip #2 Turn Laser Mode On Automaticall

If you're like me you forget to turn laser mode on/off with the $32 command. So I put it in my post processor to do it automatically. I will say you need CNCjs to make this work and will explain why later. I put the following stuff in my post process (section labels included)

begin HEADER
"$32=1"
"%wait"

begin FOOTER
"M5"
"$32=0"
"%wait"

Obviously the $32=1 turns laser mode on and the $32=0 turns it off. I also altered my non-laser post processors to include a $32=0 in their headers to make sure the laser mode is off for those. Now this only works for CNCjs for a few reasons. (1) Some versions of Carbide Motion don't like the $32 in the gcode. (2) You need the "%wait" directive that CNCjs supports. You need this because the $32 command writes to NVRAM and the controller pauses a second doing it following gcode commands are sent to the controller and lost while the write is going on. The "%wait" in CNCjs command tells CNCjs to wait until the $32 is done before proceeding. Without the "%wait" things screw up or hang. And if you're wondering if a "G4 P1" will work; it won't since it's GCODE processed by the controller.

Tip #3 Quit resetting XY zero for your Laser

I have a spindle mounted laser and the offset between the cut with a v-bit and the laser is off by 0.5mm (I think due to tramming errors). That's pretty small but I wanted 0 error so I developed a technique to reduce it to 0. And this technique will work even is your laser is offset by a large amount (like you're using a magnetic mount).

I was cutting patterns with V-Bits and wanted to mount my laser, zero Z like any other bit change, and proceed to burn a pattern that was registered on the previous cuts. I then stumbled on the G92 set of GRBL commands with allow a temporary offset to be set in place. Here is my Header section of my Laser PostProcessor with the commands included.

1 begin HEADER
2 "(Starting Program and turning Laser Mode On)"
3 "$32=1"
4 "%wait"
5 "T42"
6 "G17"
7 "G21"
8 "G90"
9 "G92.1"
10 "G0[ZH]"
11 "G0[XH][YH]"
12 + Now apply a temporaty 0.5mm offset for my laser alignment
13 "G92 X-0.5Y0.5"

So lines 1 thru 8 are pretty standard (see my tip #2 above for lines 3 & 4). The magic starts happening at line 9 which resets any temporary offset that might still be in place. Line 10 & 11 move to true 0 in case an offset was in place. Line 13 implements a new offset of X and Y values and should be whatever values your laser dot differs from your spindle cut. I carve a simple v-carve + and them laser a + and see how different you are. Then keep tweaking them until they align perfectly. You laser toolpaths will then align perfectly with your cuts. Your values for Line 13 will likely be very different than mine.

One more thing. Put the following lines in your Footer section of your laser toolpaths to turn off the offset. I also put them in the Header section of my non-laser post processors so even if a laser toolpath does not complete the offet is removed before making a cut.

+ Reset any offsets in place
"G92.1"

Well that's it for now. These are somewhat advanced concepts and may take you some time to play with and hopefully improve them
Gary Mitchell
Kentucky, USA

wb9tpg
Vectric Craftsman
Posts: 297
Joined: Tue Sep 04, 2018 2:49 pm
Model of CNC Machine: Shapeoko 3 XL

Re: How to line up JTech to home position

Post by wb9tpg »

I thought I'd take a few minutes to write up a some of my Postprocessor tips regarding using a J-Tech laser with Vcarve (or Aspire). I use a Shapeoko which is a GCODE machine.

Tip #1 No Z
I have two post processors I use with my laser. One has Z motion and the other removes the Z. An easier way to make the NO Z postprocessor is to copy the postprocessor and change this like in it to include a scale factor.

VAR Z_HOME_POSITION = [ZH|A|Z|1.3|0.00001]

The last portion of that entry take any Z entry and multplies it by 0.00001 which effectively removes it. Just zero your Z axis so your laser is 1/8" above the work surface and your good to go.

Tip #2 Turn Laser Mode On Automaticall

If you're like me you forget to turn laser mode on/off with the $32 command. So I put it in my post processor to do it automatically. I will say you need CNCjs to make this work and will explain why later. I put the following stuff in my post process (section labels included)

begin HEADER
"$32=1"
"%wait"

begin FOOTER
"M5"
"$32=0"
"%wait"

Obviously the $32=1 turns laser mode on and the $32=0 turns it off. I also altered my non-laser post processors to include a $32=0 in their headers to make sure the laser mode is off for those. Now this only works for CNCjs for a few reasons. (1) Some versions of Carbide Motion don't like the $32 in the gcode. (2) You need the "%wait" directive that CNCjs supports. You need this because the $32 command writes to NVRAM and the controller pauses a second doing it following gcode commands are sent to the controller and lost while the write is going on. The "%wait" in CNCjs command tells CNCjs to wait until the $32 is done before proceeding. Without the "%wait" things screw up or hang. And if you're wondering if a "G4 P1" will work; it won't since it's GCODE processed by the controller.

Tip #3 Quit resetting XY zero for your Laser

I have a spindle mounted laser and the offset between the cut with a v-bit and the laser is off by 0.5mm (I think due to tramming errors). That's pretty small but I wanted 0 error so I developed a technique to reduce it to 0. And this technique will work even is your laser is offset by a large amount (like you're using a magnetic mount).

I was cutting patterns with V-Bits and wanted to mount my laser, zero Z like any other bit change, and proceed to burn a pattern that was registered on the previous cuts. I then stumbled on the G92 set of GRBL commands with allow a temporary offset to be set in place. Here is my Header section of my Laser PostProcessor with the commands included.

1 begin HEADER
2 "(Starting Program and turning Laser Mode On)"
3 "$32=1"
4 "%wait"
5 "T42"
6 "G17"
7 "G21"
8 "G90"
9 "G92.1"
10 "G0[ZH]"
11 "G0[XH][YH]"
12 + Now apply a temporaty 0.5mm offset for my laser alignment
13 "G92 X-0.5Y0.5"

So lines 1 thru 8 are pretty standard (see my tip #2 above for lines 3 & 4). The magic starts happening at line 9 which resets any temporary offset that might still be in place. Line 10 & 11 move to true 0 in case an offset was in place. Line 13 implements a new offset of X and Y values and should be whatever values your laser dot differs from your spindle cut. I carve a simple v-carve + and them laser a + and see how different you are. Then keep tweaking them until they align perfectly. You laser toolpaths will then align perfectly with your cuts. Your values for Line 13 will likely be very different than mine.

One more thing. Put the following lines in your Footer section of your laser toolpaths to turn off the offset. I also put them in the Header section of my non-laser post processors so even if a laser toolpath does not complete the offet is removed before making a cut.

+ Reset any offsets in place
"G92.1"

Well that's it for now. These are somewhat advanced concepts and may take you some time to play with and hopefully improve them
Gary Mitchell
Kentucky, USA

Post Reply