What do I need to do to make Easel GCode work?

[jkendall]

My day is off to a rough start. I spilled coffee on my laptop and killed the thing. Also, I made something simple in Easel and tried running it. 

The X and Y axis went WAAAAAY off the work piece and the Z axis did a straight nosedive into the bed.

I did reset zero prior to the run, but every axis is acting as if it's in business for itself. What do I have to do to make the code work or better yet, what am I missing?

[aforww]

Did you check out this thread? Are you sending to the machine with easel or just getting the Gcode?

[jkendall]

Which thread?

And I exported the gcode.

[Derek the Admin]

Post the g code please and let's see if anything is off there.

[Derek the Admin]

Also have you tried to run the MillRight CNC engraving found on the quick start guide on theresources page?

[jkendall]

Here is where it does the nosedive:
G90
G21
G28
G21 G38.2 Z-71 F80
G10 L20 P1 X17 Y-12.25 Z12.7
G54
G0 Z20
G0 X20 Y20
M3 S12000
G0 X44.162 Y114.033
G1 Z-1.016 F228.6
G1 X43.797 Y114.219 F609.6
G1 X42.852 Y115.033 F609.6
G1 X42.454 Y115.766 F609.6
G1 X42.454 Y109.185 F609.6
G1 X44.162 Y114.033 F609.6
G1 X43.355 Y107.596 F609.6
G1 X43.404 Y108.062 F609.6
G1 X45.852 Y115.009 F609.6
G1 X44.975 Y115.076 F609.6
G1 X44.539 Y115.250 F609.6
G1 X43.824 Y115.849 F609.6
G1 X43.419 Y116.687 F609.6
G1 X43.356 Y117.153 F609.6
G1 X43.355 Y148.530 F609.6
G1 X41.184 Y148.530 F609.6
G1 X41.184 Y81.777 F609.6
G1 X43.355 Y81.777 F609.6
G1 X43.355 Y107.596 F609.6
G1 Z3.810 F228.6
G0 X49.856 Y118.439

Mar 11, 2017 19:29:53 GMT Derek the Admin said:

Also have you tried to run the MillRight CNC engraving found on the quick start guide on theresources page?

I just did. It's definitely not for pine. 

[aforww]

Mar 11, 2017 18:56:57 GMT jkendall said:

Which thread?

And I exported the gcode.

Oops, forgot the link. Sorry. millrightcnc.proboards.com/thread/180/milling-wrong?page=2

[jkendall]

I have seen that thread. I'll give it another go with the info Andrew posted. But right now I'm off to the Homeless Despot for some MDF to run the test file to make sure everything is in working order.

[mp4doggie]

Hey JK make sure when you are in UGS that when you press it is moving in the correct direction

With me my wires although where right , it was not moving the correct way


When you click X+ in UGS, does the tool move to the right?
When you click Y+ in UGS, does the bed move towards the front of the machine?... Such that the bed is hanging over the front of the machine?

[Derek the Admin]

Why do you say it isn't for pine? I think there is a picture of the results and it's actually a piece of stained pine.

Ok, so here are the issues with that code, in the order in which I find them:

1)
G28: If you have not homed and set an intermediate position with G28.1 then the G28 position may be anywhere. You either need to set the G28 position with G28.1 command or delete it from the code altogether.

Here is a great link that will explain the G28 concept.

2)
G21 G38.2 Z-71 F80:
G21 is just telling it you are using millimeters. G38.2 Z-71 F80 is telling it to probe downward all the way to -71 Z at a rate of 80mm/m until the probe pin receives a contact signal. I'm not even sure that grbl 0.9f (which is what we are using as firmware) is even going to respond to this command, but if it does then it would explain a slow nosedive.

3)
G10 L20 P1 X17 Y-12.25 Z12.7:
This command is setting the G54 work coordinate system to +17 X, -12.25 Y, and 12.7 Z from where the point you are at right now.

4)
G54:
This now selects the G54 coordinate system that was set by the G10. What you were calling Z zero, for instance, it is now calling Z 12.7.

The code had plenty of bad surprises. I'm sure other guys that we into Easel will be along to tell you how to suppress those from the output.

[mrbigj]

I don't know much about gcode and reading it, however, I can say that I'm using Easel and generating gcode and it's working perfectly for me. I design in Easel, generate and download the gcode, open it in UGS Platform, setup the machine, and run it. All of my projects so far have been done in Easel, as I'm still trying to learn Fusion 360. These other guys are probably on to the problem though, and they'll definitely help you get it figured out.

J

[mp4doggie]

Im with J ( thanks to Andrew) The issues I am having is because of me not clamping my wood down properly . Make sure your changing it back to MM when exporting the Gcode if your designing in inches

[jkendall]

Mar 11, 2017 20:26:38 GMT Derek the Admin said:

Why do you say it isn't for pine? I think there is a picture of the results and it's actually a piece of stained pine.

Ok, so here are the issues with that code, in the order in which I find them:

1)
G28: If you have not homed and set an intermediate position with G28.1 then the G28 position may be anywhere. You either need to set the G28 position with G28.1 command or delete it from the code altogether.

Here is a great link that will explain the G28 concept.

2)
G21 G38.2 Z-71 F80:
G21 is just telling it you are using millimeters. G38.2 Z-71 F80 is telling it to probe downward all the way to -71 Z at a rate of 80mm/m until the probe pin receives a contact signal. I'm not even sure that grbl 0.9f (which is what we are using as firmware) is even going to respond to this command, but if it does then it would explain a slow nosedive.

3)
G10 L20 P1 X17 Y-12.25 Z12.7:
This command is setting the G54 work coordinate system to +17 X, -12.25 Y, and 12.7 Z from where the point you are at right now.

4)
G54:
This now selects the G54 coordinate system that was set by the G10. What you were calling Z zero, for instance, it is now calling Z 12.7.

The code had plenty of bad surprises. I'm sure other guys that we into Easel will be along to tell you how to suppress those from the output.

I still have much to learn. I was using a cheap ballnose bit. They were a steal for $10 for a 10 pack on Amazon! But unfortunately, with the same type of bit with MDF as the material, I had the same issue. So I popped-in a $15 end mill and BAM! No issues running the test program.

I'm going to try to re-do the Easel export from scratch using Andrew's advice. If I see any of what you mentioned in the code in the new export, I'll make the appropriate adjustments and re-try.

Thanks for the info! Murphy is apparently my homeboy today.

[jkendall]

Mar 11, 2017 19:59:18 GMT mp4doggie said:

Hey JK make sure when you are in UGS that when you press it is moving in the correct direction

With me my wires although where right , it was not moving the correct way


When you click X+ in UGS, does the tool move to the right?
When you click Y+ in UGS, does the bed move towards the front of the machine?... Such that the bed is hanging over the front of the machine?

Yes and yes. I had issues with that earlier this week after getting the thing together. My Y-axis was installed backwards!

[Derek the Admin]

It's all part of the learning process. I was at the same point not all that long ago!