G Code question - New CNC router project ruined by return to home command?

[HoosierBuddy]

Guys,

I am slowly trying to school myself up on CNC using a small 3018 router I got for Christmas this year.

Last night I was cutting about my 5th project, but my first one where I was using the hand-held controller instead of the laptop. I had my design done and had Easel generate g-code which I then copied over to my hand held controller, took it out and plugged it into the machine. This was a roughing pass only. It ran the entire program, cut everything right, and I was out there watching it when it finished pulled up the bit and moved back towards home....and started cutting a new groove where there wasn't supposed to be one.

OK. This is the code where it ruined 7 hours of work:

G20
G90
G0 Z0.15000
G0 X0.00000 Y0.00000
G4 P0.1
M5

I read that code to say:

Unit Selection Inches
Absolute Coordinate mode
Rapid Raise Bit .15-inches above work piece
Rapid Move to X, Y Origin (keeping bit .15 inches above work piece)
Pause .1 Seconds
Shut off spindle

Question: Is there a problem with this code OR did my bit slip in the collet, drop down, ruin my zero, and then ruin my work?

I sure thought I had the bit plenty tight.

 

[niget2002]

What did the Z height read on the controller when you hit the e-stop? Or does your e-stop turn off the controller too?

You're reading the G-code correctly. My assumption is the bit slipped, but that usually happens while cutting not when moving across air. You could move the M5 so that it stops the bit after the G0Z command and before it starts to move back to home.

.15" isn't much clearance. I typically move my tool quite a bit out of the way when the cut is finished. I don't know where home is on your machine, but I also typically have the spindle move towards the back of the machine and stop after it's cleared the work piece. This keeps me from having to work around the gantry or move anything in order to get the work piece off the machine. But my Home was typically the front left corner of my machine.

 

[HoosierBuddy]

What did the Z height read on the controller when you hit the e-stop? Or does your e-stop turn off the controller too?

I didn't look. I just smacked the e-stop and cussed some. I'm pretty sure that shut off power to the controller too....but I'm not sure. That's the first time I've tried to use the controller.

There is some chance I can salvage the work piece, but regardless if I'm starting on the roughing cut or the final cut I will change that .15-inches to .5 inches....and tighten the bejesus out of the collet.

The last move the cutter made was from the slit with the numbers on each side of it. It pulled out of that slit and it was returning to home across the pocket, and didn't dig in until it got to part of the piece that had no material removed near the "H". I should be able to check the depth in the last thing it cut vs the program and see if it was cutting too deep there. I'll take a look at that too.



Thanks for the feedback!

 

[jkeyser14]

Guys,

I am slowly trying to school myself up on CNC using a small 3018 router I got for Christmas this year.

Last night I was cutting about my 5th project, but my first one where I was using the hand-held controller instead of the laptop. I had my design done and had Easel generate g-code which I then copied over to my hand held controller, took it out and plugged it into the machine. This was a roughing pass only. It ran the entire program, cut everything right, and I was out there watching it when it finished pulled up the bit and moved back towards home....and started cutting a new groove where there wasn't supposed to be one.

OK. This is the code where it ruined 7 hours of work:

G20
G90
G0 Z0.15000
G0 X0.00000 Y0.00000
G4 P0.1
M5

I read that code to say:

Unit Selection Inches
Absolute Coordinate mode
Rapid Raise Bit .15-inches above work piece
Rapid Move to X, Y Origin (keeping bit .15 inches above work piece)
Pause .1 Seconds
Shut off spindle

Question: Is there a problem with this code OR did my bit slip in the collet, drop down, ruin my zero, and then ruin my work?

I sure thought I had the bit plenty tight.

Was your ABS Z zero set at the table surface by accident?

 

[Innovate1]

Checking the depth of cut just before the problem should show if the bit was slipping or not - it's very unlikely to slip when not cutting. I had the bit slip in my router when cutting some hard cherry. The bit was supposed to ramp down and cut out the parts in several passes but at some point the cut got deeper and deeper until things went really south - stalled spindle, bent bit... I looked up the torque spec for the spindle nut and got a torque wrench - it's a very small machine and I was being too cautious on the torque. Tightened up to the proper torque and no more problem. Tool stick out can make this worse - make sure you have adequate tool shank in the collet. If there is a way to stop the machine without loosing axis zeros and offsets you could try that if it happens again and recheck position. Or measure how far out of the collet the tool is at the start so you can check it when something goes wrong. Sounds like the collet slipped to me.

 

[wyb2]

This is a typical Chinese 3018 with the spindle motor clamped in place? If it seems like the bit slipped but it really doesn’t seem like it should have, make sure the spindle is mounted tightly. If you forget to fully tighten the clamp hardware, the whole spindle can jump down under load without rotating noticeably (ask me how I know).

I like to set my Z 0 to the top of the workpiece whenever practical. That makes it very easy to spot if something is off with the travel/clearance heights.

Edit: Went back and actually payed attention to the g-code you posted, looks like you already do that last thing.

 

[Firebrick43]

Guys,

I am slowly trying to school myself up on CNC using a small 3018 router I got for Christmas this year.

Last night I was cutting about my 5th project, but my first one where I was using the hand-held controller instead of the laptop. I had my design done and had Easel generate g-code which I then copied over to my hand held controller, took it out and plugged it into the machine. This was a roughing pass only. It ran the entire program, cut everything right, and I was out there watching it when it finished pulled up the bit and moved back towards home....and started cutting a new groove where there wasn't supposed to be one.

OK. This is the code where it ruined 7 hours of work:

G20
G90
G0 Z0.15000
G0 X0.00000 Y0.00000
G4 P0.1
M5

I read that code to say:

Unit Selection Inches
Absolute Coordinate mode
Rapid Raise Bit .15-inches above work piece
Rapid Move to X, Y Origin (keeping bit .15 inches above work piece)
Pause .1 Seconds
Shut off spindle

Question: Is there a problem with this code OR did my bit slip in the collet, drop down, ruin my zero, and then ruin my work?

I sure thought I had the bit plenty tight.

Did you have Origin at the table surface? Or the top of the work?

 

[NHtoolguy]

When I did G Code programming years ago, one of the first lines of code established the workpiece datum from the machine datum (called a "datum shift"). This was used with the tool offset file to tell the controller where to move the tool relative to the workpiece in the machine envelope. If the datum shift or the tool offset was incorrect, crashes would occur (especially dramatic when using G0 rapid moves). We would dry run each new program using low speed "jog" mode until we knew the code was correct.

 

[niget2002]

Did you have Origin at the table surface? Or the top of the work?

That shouldn't matter. He used a G0 X0 Y0, which shouldn't move Z.

 

[Firebrick43]

That shouldn't matter. He used a G0 X0 Y0, which shouldn't move Z.

The line directly above that was G0 Z0.15000. Unless it was already at z0.1500 then it did move Z.

 

[niget2002]

The line directly above that was G0 Z0.15000. Unless it was already at z0.1500 then it did move Z.

correct. Up and out the way. Then it did the G0 to move back to XY origin. Gcode will do one movement, then the next. It's not going to start the G0X0Y0 until after the G0Z0.15 completes.

 

[Firebrick43]

correct. Up and out the way. Then it did the G0 to move back to XY origin. Gcode will do one movement, then the next. It's not going to start the G0X0Y0 until after the G0Z0.15 completes.

But if he set origin at the spoil board/table instead of on top of the work then G0 Z0.15000 is highly unlikely to clear the work when it makes its x/z move

It could be also caused by resetting the program and not calling back in your work offset (such as G54), seen a few million dollar blocks scrapped due that one.

Or tool offset (G43 or tool itself) not called back in after a reset or jumping in the program.

Both of these a dependent on the controller, some clear and most don’t.

 

[HoosierBuddy]

Since I had pretty much already ruined the workpiece with the roughing pass, I went ahead and ran the detail pass too to see if any other issues popped up.

There were 2 other instances where the bit failed to raise above the workpiece on the way back to home. As a for instance, the S I show in my picture above ended up looking like a $ sign.

This time I'm 100% positive the bit didn't slip.

I bought some soft pine and am planning on retrying this with my Safety Height above the workpiece set higher like maybe 1/2". Not sure why that would help, but I'll give it a shot.

Right now I'm wondering if it's a problem with the inexpensive 3018 CNC machine. The issue doesn't appear to be in the Easel generated G Code.

I'm kind of wondering if it could be in the handheld controller even. I didn't have this issue when running directly from a laptop.

 

[niget2002]

But if he set origin at the spoil board/table instead of on top of the work then G0 Z0.15000 is highly unlikely to clear the work when it makes its x/z move

Gotcha. I was still thinking relative positioning not absolute.

 

[Firebrick43]

Since I had pretty much already ruined the workpiece with the roughing pass, I went ahead and ran the detail pass too to see if any other issues popped up.

There were 2 other instances where the bit failed to raise above the workpiece on the way back to home. As a for instance, the S I show in my picture above ended up looking like a $ sign.

This time I'm 100% positive the bit didn't slip.

I bought some soft pine and am planning on retrying this with my Safety Height above the workpiece set higher like maybe 1/2". Not sure why that would help, but I'll give it a shot.

Right now I'm wondering if it's a problem with the inexpensive 3018 CNC machine. The issue doesn't appear to be in the Easel generated G Code.

I'm kind of wondering if it could be in the handheld controller even. I didn't have this issue when running directly from a laptop.

So searching 3018 it looks like this is a very small machine with nema 17 stepper motors right?

If so you could be loosing steps from either motion issues in the ways/axis drive line, driving it too hard in the work, or a combination of both.

Sometimes when we had tolerance issues we would make a program to drive an axis 75 percent of its travel back and forth 50 times or so and see if it repeated back to the start position. We would set a 1-2-3 block up and put an indicator in the spindle.

But a small machine you can use a block and manually drive it to down to touch off with a piece of cigarette, slowly stepping down by 0.001” until the paper tears, and set g54 to zero at that point.

Program a different x y position and make a program there to move plus Z3.00 and down to Z0.0 and repeat 50 times. End with z up at 3.00, reset, and manually drive back over your block and slowly use the hand wheel to bring it back to touch off the block. The cigarette paper should tear at the same point.

 

[wyb2]

Since I had pretty much already ruined the workpiece with the roughing pass, I went ahead and ran the detail pass too to see if any other issues popped up.

There were 2 other instances where the bit failed to raise above the workpiece on the way back to home. As a for instance, the S I show in my picture above ended up looking like a $ sign.

This time I'm 100% positive the bit didn't slip.

I bought some soft pine and am planning on retrying this with my Safety Height above the workpiece set higher like maybe 1/2". Not sure why that would help, but I'll give it a shot.

Right now I'm wondering if it's a problem with the inexpensive 3018 CNC machine. The issue doesn't appear to be in the Easel generated G Code.

I'm kind of wondering if it could be in the handheld controller even. I didn't have this issue when running directly from a laptop.

You just reminded me of a problem I had with my 3020 where it would randomly freeze mid-program with the spindle still running. It was extremely irritating because it would lose home when this happened, so any variation when I re-zeroed would carry through rerunning the program. This was running via a USB cable from the laptop using Candle.

I eventually tracked it down to EMI interference from the spindle motor to the USB cable. Luckily something was recognizing a problem and causing the program to stall, instead of executing gibberish. I changed my setup so the USB cable doesn’t route anywhere near the spindle power wires, and the problem disappeared.

I wonder if interference could be causing lost commands/steps.

 

[Firebrick43]

You just reminded me of a problem I had with my 3020 where it would randomly freeze mid-program with the spindle still running. It was extremely irritating because it would lose home when this happened, so any variation when I re-zeroed would through rerunning the program. This was running via a USB cable from the laptop using Candle.

I eventually tracked it down to EMI interference from the spindle motor to the USB cable. Luckily something was recognizing a problem and causing the program to stall, instead of executing gibberish. I changed my setup so the USB cable doesn’t route anywhere near the spindle power wires, and the problem disappeared.

I wonder if interference could be causing lost commands/steps.

That’s a real possibility. Most real machines use shielded cable with the shield attached to the ground plane in the cabinet to drain any interference. I have seen axis do the funky chicken before and found the shield unhooked and attaching it solved the issue. Ferrite chokes may also signal wires reject interference

 

[HoosierBuddy]

I tried again last night and about 40 minutes in the router took off across the piece again ruining another project. I sent a picture off to the manufacturer and asked them what to do.

They said to check the z-axis motor up and down manually to make sure it's not binding (it's not). If that's OK they told me how to adjust the current supplied from the controller to the z--axis motor to increase it. I'll try that later today.

The other thought I've had on this...see if any of you think this might be a good idea? Open the g-code in my text editor and do a global search and replace to change all the G0 Z1.0000 commands (rapid move to safe distance above piece) to G1 Z1.0000 commands (Normal move to safe distance above piece). The only issues I'm having are with the G0 commands....so maybe just get rid of all of them???

 

[Firebrick43]

What is your rapid speed?

There usually is a way to set it in the controller or you can make it modal by adding a F command to your first G0 command

G0 Z0.1500 F150

This would set the feed rate to 150 inches per min modal and therefore all other other G0 commands would be the same further down in the program.

It looks like the max speed of some 3018 is 5000mm/m feed rate which if my math is correct is 196 inches per min, which is why I picked 150 but it may need slowed furthre?

There is also accel/deaccel rates in the controller that should be able to be adjusted but I have no idea what controller you have.

Why this is important.

Steeper motors are usually **** on but they actually have really high torque at low speeds, much better than servos motors, especially without the reduction drives they usually have on them. HOWEVER they loose torque once you start speeding up. I depends on the size of the the motor. Servos however perform well at speed, and with gear reductions can exceed steppers performance at nearly any speed but are very expensive.



You can see by the chart above that has several different length Nema 17 motors on it that after 1500 rpms they have lost half of their torque output. If you drive into this region the motors are likely to loose steps because they physically dont have the torque to complete the movement and without encoders on the motor have no idea that they have not actually completed the movement.

 

[HoosierBuddy]

What is your rapid speed?

There usually is a way to set it in the controller or you can make it modal by adding a F command to your first G0 command

G0 Z0.1500 F150

This would set the feed rate to 150 inches per min modal and therefore all other other G0 commands would be the same further down in the program.

It looks like the max speed of some 3018 is 5000mm/m feed rate which if my math is correct is 196 inches per min, which is why I picked 150 but it may need slowed furthre?

There is also accel/deaccel rates in the controller that should be able to be adjusted but I have no idea what controller you have.

Why this is important.

Steeper motors are usually **** on but they actually have really high torque at low speeds, much better than servos motors, especially without the reduction drives they usually have on them. HOWEVER they loose torque once you start speeding up. I depends on the size of the the motor. Servos however perform well at speed, and with gear reductions can exceed steppers performance at nearly any speed but are very expensive.



You can see by the chart above that has several different length Nema 17 motors on it that after 1500 rpms they have lost half of their torque output. If you drive into this region the motors are likely to loose steps because they physically dont have the torque to complete the movement and without encoders on the motor have no idea that they have not actually completed the movement.

Great info.

I'll edit the first GO command as you suggest....maybe even be a lot more conservative to see if that corrects the issue.

The only thing that's got me super confused with this scenario is why does the z position seem ok for subsequent cutting after the missed Z0 commands? Meaning....if the controller tells the steeper "Go up an inch" and it can't/doesn't" seems like it would move over and then plunge an inch? Are we saying it's trying to do that but as it's still in rapid mode for that move it ALSO doesn't have the torque to plunge cut at rapid speed into pine?

 

[Firebrick43]

Great info.

I'll edit the first GO command as you suggest....maybe even be a lot more conservative to see if that corrects the issue.

The only thing that's got me super confused with this scenario is why does the z position seem ok for subsequent cutting after the missed Z0 commands?

It shouldn’t be with steppers, once you loose steps you are screwed.

Meaning....if the controller tells the steeper "Go up an inch" and it can't/doesn't" seems like it would move over and then plunge an inch?

It would plunge an inch from where ever it is at that moment because it has no way of knowing it has lost motion

Are we saying it's trying to do that but as it's still in rapid mode for that move it ALSO doesn't have the torque to plunge cut at rapid speed into pine?

Definitely wouldn’t have torque to plunge at rapid speeds.


I am still concerned about how you are finding your origin? Spoils plate or top of work? Setting program zero there or setting a work offset of G54, G55, ect?

 

[HoosierBuddy]

I am still concerned about how you are finding your origin? Spoils plate or top of work? Setting program zero there or setting a work offset of G54, G55, ect?

I'm moving it to the front left top point of the work piece. for 0,0,0. For the top, I get it close and then manually adjust it with the hand wheel on the z axis until a piece of paper can barely be pulled under the bit. On the x and y, I lay a flat edge against the side of the piece and use the hand wheels to manually get it until it exactly touches the flat edge.

 

[Firebrick43]

Most of these routers use a version of a 3D printer control board and their base firmware.

Do you know what board and if it’s running Marlin, RepRap, or Klipper?

Also can you post a picture of the first page or two of a programs gcode? Just the preparatory code and a few lines down to where it starts cutting

 

[HoosierBuddy]

I'll look at the board and see what I can figure out.

This is the start of the code for the rough pass:

G20
M3 S12000
G90
G1 Z1.00000 F9.0
G0 X1.03409 Y0.67795
G1 Z-0.06250 F9.0
G1 X1.04984 Y0.68448 F40.0
G1 X1.06207 Y0.69672 F40.0
G1 X1.06860 Y0.71246 F40.0
G1 X1.06863 Y0.72980 F40.0
G1 X1.06213 Y0.74557 F40.0
G1 X1.04984 Y0.75790 F40.0
G1 X1.03409 Y0.76443 F40.0
G1 X1.01666 Y0.76443 F40.0
G1 X1.00095 Y0.75790 F40.0
G1 X0.98865 Y0.74570 F40.0
G1 X0.98209 Y0.72980 F40.0
G1 X0.98212 Y0.71246 F40.0
G1 X0.98865 Y0.69675 F40.0
G1 X1.00095 Y0.68448 F40.0
G1 X1.01666 Y0.67795 F40.0
G1 X1.03409 Y0.67795 F40.0
G0 Z0.00000
G1 X1.03079 Y0.69412 F40.0
G1 Z-0.12500 F9.0
G1 X1.04068 Y0.69821 F40.0

Etc......

 

[HoosierBuddy]

So...I'm now 100% convinced this is all hardware related and specifically the z-axis motor and or controller.

I turned the screw the customer service tech told me to turn one turn clockwise and that locked up the z axis completely. When I tried to move the z with the handheld controller it would just whine. I put it about half way back to where it started and it would work in a jerky fashion. I put it all the way back to where I started and now the z axis would move up and down as expected.

I don't understand why this seems to be working exactly opposite of what their tech told me would happen.

In any case, I then used a text editor to change all of my G0 moves to a safe height to G1 Z1.00000 F40.

That slowed down the operation slightly, but I ran the entire roughing cut with no issues.

For whatever reason my z-motor is not able to consistently handle the rapid moves.

I sent an email back to tech support and told them when I turned the adjustment screw in it just locks the z axis. I'll see what their response is.

 

[wyb2]

So...I'm now 100% convinced this is all hardware related and specifically the z-axis motor and or controller.

I turned the screw the customer service tech told me to turn one turn clockwise and that locked up the z axis completely. When I tried to move the z with the handheld controller it would just whine. I put it about half way back to where it started and it would work in a jerky fashion. I put it all the way back to where I started and now the z axis would move up and down as expected.

I don't understand why this seems to be working exactly opposite of what their tech told me would happen.

In any case, I then used a text editor to change all of my G0 moves to a safe height to G1 Z1.00000 F40.

That slowed down the operation slightly, but I ran the entire roughing cut with no issues.

For whatever reason my z-motor is not able to consistently handle the rapid moves.

I sent an email back to tech support and told them when I turned the adjustment screw in it just locks the z axis. I'll see what their response is.

But didn’t you state earlier that the Z heights seem correct after the failed rapid up? As I think others have pointed out, once you loose steps that were sent to the motor you at screwed, the delta will carry forward. Seems to me like it’s not hardware related and there is a software issue with sending the GO command.

I think you also said this hasn’t happened with the laptop, so definitely seems to point to the handheld controller skipping that GO command for some reason.

 

[HoosierBuddy]

But didn’t you state earlier that the Z heights seem correct after the failed rapid up? As I think others have pointed out, once you loose steps that were sent to the motor you at screwed, the delta will carry forward. Seems to me like it’s not hardware related and there is a software issue with sending the GO command.

I think you also said this hasn’t happened with the laptop, so definitely seems to point to the handheld controller skipping that GO command for some reason.

If the motor doesn't have the nuts to rapid UP it definitely doesn't have the power to plunge cut during a rapid down. It ends up approximately back where it started (In the Z-axis) by not moving up and then not moving down during 2 successive rapid z moves. By eliminating the rapid moves and doing those slow, the stepper motor has more torque (See FireBrick above) and that seems to get me a good cut. I don't think this is a great long term solution as it requires me to edit all my g-code before cutting with it.

 

[wyb2]

If the motor doesn't have the nuts to rapid UP it definitely doesn't have the power to plunge cut during a rapid down. It ends up approximately back where it started (In the Z-axis) by not moving up and then not moving down during 2 successive rapid z moves. By eliminating the rapid moves and doing those slow, the stepper motor has more torque (See FireBrick above) and that seems to get me a good cut. I don't think this is a great long term solution as it requires me to edit all my g-code before cutting with it.

I guess it’s possible. On the way down it would have the weight of Z carriage and spindle helping rather than fighting the motor, so I would think you would be able to see/hear it attempting to plunge.

Can you adjust machine settings (max speed) in Easel? That might save you having to manually edit the g-code. If you want to investigate further, maybe create program of just Z travels up and down of increasing speed and see when things go awry.

 

[whateg01]

What do you mean by halfway through the job, it took off across the work? That doesn't sound related to z at all.

I will often cut air the first time I run a program of I think there might be areas of concern. With you having problems, I would do that before ruining more work, although if it's just common lumber, I guess it's no big deal.

 

[Firebrick43]

If the motor doesn't have the nuts to rapid UP it definitely doesn't have the power to plunge cut during a rapid down. It ends up approximately back where it started (In the Z-axis) by not moving up and then not moving down during 2 successive rapid z moves. By eliminating the rapid moves and doing those slow, the stepper motor has more torque (See FireBrick above) and that seems to get me a good cut. I don't think this is a great long term solution as it requires me to edit all my g-code before cutting with it.

They don't look too complicated.

I would suggest removing the motor and unhooking the z axis screw and make sure that the guide rods and corresponding bushings are free without binding or cocking with the cantilevered weight of the router motor.

Once you have eliminated the linear motion from faults then more than likely its either the screw itself, turn by finger to see if it binds in specific places. I would assume that it has some kind of double nut or backlash compensation on the nut? They can cause issues as well if the springs are not in place correctly or just poor quality.

The thrust bearing at the bottom can also fail. Of course it can be the stepper motor but you could see if it has issues unhooked after testing the other components.

 

[jkeyser14]

Since I had pretty much already ruined the workpiece with the roughing pass, I went ahead and ran the detail pass too to see if any other issues popped up.

There were 2 other instances where the bit failed to raise above the workpiece on the way back to home. As a for instance, the S I show in my picture above ended up looking like a $ sign.

This time I'm 100% positive the bit didn't slip.

I bought some soft pine and am planning on retrying this with my Safety Height above the workpiece set higher like maybe 1/2". Not sure why that would help, but I'll give it a shot.

Right now I'm wondering if it's a problem with the inexpensive 3018 CNC machine. The issue doesn't appear to be in the Easel generated G Code.

I'm kind of wondering if it could be in the handheld controller even. I didn't have this issue when running directly from a laptop.

The stepper motor could be stalling/losing steps. You may need to slow down the z-axis and also check for binding.

 

[HoosierBuddy]

I ran the finish pass on the part I'd (FINALLY) successfully run a rough pass (after editing all the G code to slow down z axis travel). I made the same changes to the finish pass. It was made using a 30-degree engraving bit.

I started it running and went to work. When I came home the engraving bit was buried into the workpiece to the depth of the collet and the machine had stalled at that point. Luckily where the bit was buried was centered over one of the slots in the table, so it didn't get into the aluminum.

I mean....the router is brand new. It doesn't work. With all of y'all's help I'm sure the G-Code isn't the issue. The machine doesn't work right or even consistently screw-up at the same point. I'm dealing with Yunlee customer support and we'll see what they say. I think I need parts. Maybe a new stepper motor. Maybe a new controller. Maybe a new machine. They sent me some test code to run to see what happens. I feel like I'm just going to be jumping through whatever hoops they set up to diagnose the issue and then (hopefully) they'll send me what I need to get this thing working right.

 

[whateg01]

I started it running and went to work. When I came home the engraving bit was buried into the workpiece to the depth of the collet and the machine had stalled at that point. Luckily where the bit was buried was centered over one of the slots in the table, so it didn't get into the aluminum.

Why on FSM's green earth would you start a machine that has been problematic and then go to work?????????? Seems like a good way to come home to a smouldering pile of ash!

I mean....the router is brand new. It doesn't work. With all of y'all's help I'm sure the G-Code isn't the issue. The machine doesn't work right or even consistently screw-up at the same point. I'm dealing with Yunlee customer support and we'll see what they say. I think I need parts. Maybe a new stepper motor. Maybe a new controller. Maybe a new machine. They sent me some test code to run to see what happens. I feel like I'm just going to be jumping through whatever hoops they set up to diagnose the issue and then (hopefully) they'll send me what I need to get this thing working right.

These little machines, like many cheap 3d printers are not good for people who don't have the ability to troubleshoot and tinker. Maybe you need to spend the coin on a better turn key solution but it's going to be more expensive.

 

[wyb2]

These cheap machines exist on a spectrum between a complete working machine out of the box and a kit of parts. If customer service helps you, that’s great. But I wouldn’t rely on it at this price point.

The problems being inconsistent, I would look for loose connections and potential EMI issues.

 

[HoosierBuddy]

These cheap machines exist on a spectrum between a complete working machine out of the box and a kit of parts. If customer service helps you, that’s great. But I wouldn’t rely on it at this price point.

The problems being inconsistent, I would look for loose connections and potential EMI issues.

Yeah. Agree. I've looked and all the connectors are seated firmly but it's possible something in a connector is not making good contact.

I've got the router set up running test code customer service sent me right now. It's just "cutting" air. I believe the goal is to have it run around for a while, then return to home and see if it's lost itself. The email I got from them just said "Run this and report back"...so not 100% sure what the goal is.

 

[niget2002]

Never leave a CNC running when you leave the room. Much less the house.

In the event the router bit gets stuck in the wood, the bit rubbing the wood can and has started fires in people's garages. There's a running thread in another forum I'm on with photos of people's burned projects where they stepped away for two seconds and had to put a fire out.

I've had to pour Mt Dew on work pieces before and I was standing right there when it happened (bad feed rate in MDF causing bit to heat up).

You got lucky.

 

[HoosierBuddy]

Why on FSM's green earth would you start a machine that has been problematic and then go to work?????????? Seems like a good way to come home to a smouldering pile of ash!


These little machines, like many cheap 3d printers are not good for people who don't have the ability to troubleshoot and tinker. Maybe you need to spend the coin on a better turn key solution but it's going to be more expensive.

It's sitting on my steel router table in the middle the concrete floor in my barn. It'll be OK.

The big goal, as I think I stated earlier in this thread, is to get a feel for designing work in 2.5 or 3 D, generating g code, and producing small useful projects while climbing the learning curve needed to utilize these types of machines (routers, engravers, 3d printers even). Then, if I have interest and have come up with bigger/better ideas for projects, in an ideal world I'd upgrade to a better machine. I've got big manual machines now for large projects, but I can't, you know, do lettering or whatever on my knee mill.

I think you may have hit on a big flaw in my plan though, If these cheap 3018 machines are not really "functional", I'm not giving the whole CNC hobby a fair shake. The machine I bought has good reviews. I'm hoping they can help me get it working reliably.

I've learned a fair amount so far....but i pretty much stuck until I can get this machine working right.

 

[whateg01]

Never leave a CNC running when you leave the room. Much less the house.

In the event the router bit gets stuck in the wood, the bit rubbing the wood can and has started fires in people's garages. There's a running thread in another forum I'm on with photos of people's burned projects where they stepped away for two seconds and had to put a fire out.

I've had similar. Except I stepped away for about 30 seconds, got distracted, and it ended up being about 5 minutes. No real harm but lots of smoke. Could have gotten worse if I hadn't returned.

You got lucky.

Nothing bad ever happens... Until it does.

 

[gte718p]

It's sitting on my steel router table in the middle the concrete floor in my barn. It'll be OK.

The big goal, as I think I stated earlier in this thread, is to get a feel for designing work in 2.5 or 3 D, generating g code, and producing small useful projects while climbing the learning curve needed to utilize these types of machines (routers, engravers, 3d printers even). Then, if I have interest and have come up with bigger/better ideas for projects, in an ideal world I'd upgrade to a better machine. I've got big manual machines now for large projects, but I can't, you know, do lettering or whatever on my knee mill.

I think you may have hit on a big flaw in my plan though, If these cheap 3018 machines are not really "functional", I'm not giving the whole CNC hobby a fair shake. The machine I bought has good reviews. I'm hoping they can help me get it working reliably.

I've learned a fair amount so far....but i pretty much stuck until I can get this machine working right.

I still wouldn't leave it. Routing makes a lot of saw dust. Even small parts make a huge mess. It can go sideways fast. You do you, but you've been warned.

In any case, the cheap 3018 and related small machines are very functional. That is not the same as easy. If you master the fundamentals on them, you will be setup for any machine in the future. I have done tons of work with mine. I am currently re-designing the head because I don't like the design, but I find it incredibly useful to have around for small things. Because of the open bed, I can engrave things that don't fit in the enclosed laser.

Like others have said, I would absolutely check the collet is tight. Those little ones are notorious for coming loose. Give it a good once over that is actually the correct size, is round and not an oval, and there are no burs. If the collets are not sized correctly, they will slip when they get hot. Torquing them down will not help. They can feel tight and the bit seems solid, but after running for a few minutes, the tool slips out. Ask me how I know.

Check all connections.

Make sure all the bolts are tight on the machine. Then, profile the machine. Make sure it is square and the bed is the same distance from the head at all points along the travel. Sadly, a tenth of an inch is well inside the acceptable tolerance for these machines. Plenty of Youtube videos on how to do this. You are not doing a .00001 machining center so a test indicator is not necessary. A dial indicator is nice, but even that is not an absolute necessity.

Make sure the head is moving up and down smoothly. It is a crappy design and they like to bind. Especially on fast moves you can lose steps causing absolute position to drift. There is no error checking on these little GRBL machines. Slow feeds way down. This can also help with EMI issues.

.15 inches is not a lot of room for error on a system as flexible as a 3018. Go big on safety factors. .5 or 1 inch.

These machines will never hold tenths in the machinist meaning of the world. However, they should be able to make good parts. You should be able to repeatably get to .05 inches.

 

[HoosierBuddy]

An update guys.

My original question was related to if the code was causing the crash. It wasn't.

The manufacturer doesn't seem to have a lot of faith in their offline controller. They told me not to use it for complex parts. Not sure how/what is a "complex part"....so I went back to running it off my laptop using easel.

That got me from 100% scrap down to about 33% scrap. The last issue I had was with a small coaster I was cutting. The first 2 I made went fine. The third one made it to about 75% of the detail cut (about 2 hours in) and then just took off in the +y until it hit the limit. I contacted the manufacturer and Easel.


Bottom of Coaster. These get flipped and the top cut as well to make round, stackable coasters. I raised the cutter manually to take this photo, but the table has not been moved from where it ended the cut. See gouge.

Easel felt the issue looked like interference/noise in the USB connection. They suggested verifying the USB cable has a ferrite choke (it does), routing the USB cable away from any electrical noise, and strongly suggested using a USB Hub rather than a direct connection.

I have not bought such a hub yet. Does anyone know why this would be? They didn't provide a reason.

The router manufacturer said the issue was likely using Easel to run the router. As easel is cloud based, they felt a network connectivity issue could be to blame.

I cut some new stock, set everthing up with all suggestions (except the USB hub...as I don't have one yet), used Universal G Code sender rather than Easel to control the machine, and was able to finish my 4 coasters (cutting on both front and back) with no further issues.

I've got one more project in the hopper. It's somewhat complicated. I guess I'll try it using the the UGS and see how it goes.

So, regarding watching the router...I'm curious if you guys tweak your cut speeds or use larger bits? Each of these coasters requires a rough pass on the bottom, a detail pass on the bottom, get flipped over, the front takes a rough pass, a detail pass, then an outline pass to cut it out (except the 4 tabs). Total cut time per coaster is about 5 or 6 hours. I made 4 plus a prototype that I had to reject because it wouldn't stack right, plus one I cut out of pine to see how it looked. Say 30 to 35 hours of cut time to make 4 coasters. I mean...I get what you're saying about watching the machine....but if I had to sit on a stool for almost a full work week to make 4 coasters? Just isn't going to happen.