How to line up JTech to home position

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: 1450
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 Wizard
Posts: 453
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 Wizard
Posts: 453
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 Wizard
Posts: 453
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 Wizard
Posts: 453
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

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 928
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: How to line up JTech to home position

Post by Tex_Lawrence »

wb9tpg wrote:
Tue May 04, 2021 2:01 am
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).
Thank you, Gary. Due to a benevolent benefactor, I'm finally installing a J-Tech 7W laser magnet mount. With your post processor details, I should be able to get beyond the ubiquitous "HELLO WORLD" example! :D

With J-Tech's docs suggesting it, I downloaded UGS, but haven't even unpacked it yet. LB won't run on the little tablet (RCA) that I bought to run Carbide Motion (something about "Itanium processor"), so I'm going to have to add some sender to that tablet. CNCjs seems to be the popular one with you and those folks at the C3D forum and that's good enough for me.

PS. LB will run on my PC, but I'll need a 20 foot USB cable to connect! :D I do have a Windows laptop that I could press into service, but that reverses all of the load the file and go at my Shapeoko.
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 928
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: How to line up JTech to home position

Post by Tex_Lawrence »

wb9tpg wrote:
Tue May 04, 2021 2:01 am
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.
Gary, I haven't found the reference to explain what the "1.3" parameter is in your variable above. The PP that comes from JTECH has "1.4" in that line. (Of course, they just comment out all Z moves anyway.)

I'm trying to merge your experienced PP with the one JTECH supplies.

Thanks in advance!
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

wb9tpg
Vectric Wizard
Posts: 453
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 »

1.3 is the precision. The 3 shows how many numbers after the decimal point. For my Shapeoko CNC it has 40 steps for mm so each step is 0.025mm. I determined adding another digit to that would not affect where the CNC actually positioned. You can change it to 4 if you want. 3 works well with GRBL ARC commands too (some people had issues with 1.4 IIRC)

Now for a post processor using Inches you need more precision

Funny I do the majority of the designs in inches but use exclusively use my own modified mm post processors.

That answer your question?
Gary Mitchell
Kentucky, USA

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 928
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: How to line up JTech to home position

Post by Tex_Lawrence »

Precision! Something I deal with in spreadsheets all the time, but its so hidden there.

Now I think I can move on. I’m kind of enjoying being a newbie at something again!

Gary, your tip on the offset setting makes this Vectric software useable. The Vectric laser tutorials are really just demonstration videos.
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

wb9tpg
Vectric Wizard
Posts: 453
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 »

So did you get your offset calibrated?

I made a test pattern of a circle with a plus in the middle. I profiled it with a v bit very very shallow.

Then lasered the plus. I offset the circle vector so the laser was just outside the engraved circle. A few tries and you can nail it

If Vectric made a small change to the post processor I could do both laser and bits in a single pp
Gary Mitchell
Kentucky, USA

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 928
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: How to line up JTech to home position

Post by Tex_Lawrence »

wb9tpg wrote:
Sat Jul 10, 2021 3:23 pm
... If Vectric made a small change to the post processor I could do both laser and bits in a single pp
I thought this was the post processor. You mean something else? What change could they make, besides adding a way to make offsets tool specific?

I haven't started the calibration yet. I'm busy trying to shoehorn a 7'x30"x27" pantry cabinet into my kitchen. :shock:
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

wb9tpg
Vectric Wizard
Posts: 453
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 use 3 post processors - two for laser and one for everything else. I'd need to J-tech to allow a separate header sections for laser and other to do it all in one post processor.

And a actually have two different laser post processors - one does not have Z movement.
Attachments
Grbl_mm_V2.pp
(8.3 KiB) Downloaded 88 times
JTech_NO_Z_mm.pp
(7.84 KiB) Downloaded 103 times
Gary Mitchell
Kentucky, USA

User avatar
Tex_Lawrence
Vectric Wizard
Posts: 928
Joined: Fri Mar 25, 2016 11:30 am
Model of CNC Machine: Shapeoko3XXL; JTech7W; V-CarvePro 11.554
Location: Dayton, Texas (Don't Mess With My Texas!)

Re: How to line up JTech to home position

Post by Tex_Lawrence »

I see what you are saying, Gary, but I'm thinking that GRBL would probably be the limiting object there.

Thanks for posting your PP, because it never hurts to have more info! :D
Tex — Crooked Wood Products
Now there's a man with an open mind – you can feel the breeze from here.

Post Reply