Zero set in Aspire

[tunacnc]

I recently upgraded from Vcarve 10 to Aspire 10.5. On my first project with Aspire, I went to do a simple pocket cut to flatten a warped walnut board and I set the zero on the machine to the surface of the highest point in the board. When I started the cut, it moved the bit to the X,Y starting point and then plunged the bit about a quarter inch into the board before the spindle stopped. Trying to figure out what went wrong, I had it do a couple of fly cuts setting it about an inch above the material, each time when it starts to cut it drops it about half an inch below where I set zero. The project is only doing .05 inch deep cuts, so not sure why it's doing that. I remade the project in vCarve and it works fine, I remade the project in Aspire and it still drops about half and inch below zero.
I imported the Tool database from Vcarve 10, and I'm using the same bit and post processor. It's an Axiom Precision AR8 Pro. Any idea why there's a difference between vCarve and Aspire output files?
It's as if it was compensating for a Puck touch off for setting zero, but I'm not using one, I'm setting zero by eye.

[Rcnewcomb]

Are you using the same post-processor for both V-Carve and Aspire?

Can you attach the .CRV and the .CRV3D files so we can look at the differences?

Link -> How do I upload files or photos to the forum?


If the files are too large to upload you can put them on a site like drive.google.com or dropbox.com, make the files shareable, and share the link(s) here.

[Jim_in_PA]

Also check the material settings so they are reflective of "top of material" or "top of machine" and if that needs changed, be sure to recalculate the toolpaths. I've had this kind of thing happen myself and that invariably was where the solution was to be had.

[tunacnc]

Are you using the same post-processor for both V-Carve and Aspire?

Can you attach the .CRV and the .CRV3D files so we can look at the differences?

Link -> How do I upload files or photos to the forum?


If the files are too large to upload you can put them on a site like drive.google.com or dropbox.com, make the files shareable, and share the link(s) here.

Both are using the same post processor. I will try to upload the files.

[tunacnc]

Also check the material settings so they are reflective of "top of material" or "top of machine" and if that needs changed, be sure to recalculate the toolpaths. I've had this kind of thing happen myself and that invariably was where the solution was to be had.

I definitely set it to top of material. I rebuilt the project multiple times and literally did the exact same steps in vCarve and Aspire.

[gkas]

You should be using the "Axiom_HHC_CNC.pp"

[SteveNelson46]

Are you sure the project is set to the material surface in Aspire and the z-zero is set to the top of the material at the machine? This has happened a couple of times to me and it was usually because I got one of them wrong or one of them was changed inadvertently.

[tunacnc]

You should be using the "Axiom_HHC_CNC.pp"

There's only one Axiom post processor in the list, and its displaying as "Axiom HHC CNC (mm) (*.mmg)" That's the one I'm using.

[tunacnc]

Are you using the same post-processor for both V-Carve and Aspire?

Can you attach the .CRV and the .CRV3D files so we can look at the differences?

Link -> How do I upload files or photos to the forum?


If the files are too large to upload you can put them on a site like drive.google.com or dropbox.com, make the files shareable, and share the link(s) here.

Here are the files:

aWalnut.crv3d

Aspire version

(26 KiB) Downloaded 75 times

Vwalnut.crv

vCarve version

(24 KiB) Downloaded 65 times

[Rcnewcomb]

I looked at both files. They are not identical, so the G-code generated is slightly different between the two.

In VCarve the rectangle is 6.9262" wide by 26.0914" high. The lower left corner of the rectangle is at X-0.5881", Y -0.5457"
In Aspire the rectangle is 6.8283" wide by 26.0718" high. The lower left corner of the rectangle is at X-0.5392", Y -0.5359"
Both files have the same material size, with Z-zero on the surface of the material.
Both files show a pocket toolpath with a 0.05" depth of cut.

For both VCarve and Aspire I used the Axiom HH CNC (mm) (*.mmg) post processor.

The G code generated by both VCarve and Aspire show Z descending to -1.270mm

The code generated by VCarve was:

Code: Select all

(Filename:  VcarvePocket 1)
N10M03S12000
(Pocket 1)
N30G00X57.199Y58.275Z5.080
N40G1Z0.000F762.0
N50G1X82.599Z-0.635
N60G1X57.199Z-1.270
N70G1X88.851F2032.0
N80G1Y576.725
N90G1X57.199
N100G1Y58.275
N110G1X33.831Y34.907
N120G1X112.219
N130G1Y600.093
N140G1X33.831
N150G1Y34.907
N160G1X10.463Y11.539
N170G1X135.587
N180G1Y623.461
N190G1X10.463
N200G1Y11.539
N210G00Z5.080
N220G00Z20.320
N230M05
N240M30
%

The code generated by Aspire was:

Code: Select all

(Filename:  AspirePocket 1)
N10M03S12000
(Pocket 1)
N30G00X72.665Y72.748Z5.080
N40G1Z0.000F762.0
N50G1X73.385Z-0.018
N60G1Y97.429Z-0.635
N70G1Y72.748Z-1.252
N80G1X72.665Z-1.270
N90G1X73.385F2032.0
N100G1Y562.252
N110G1X72.665
N120G1Y72.748
N130G1X52.345Y52.428
N140G1X93.705
N150G1Y582.572
N160G1X52.345
N170G1Y52.428
N180G1X32.025Y32.108
N190G1X114.025
N200G1Y602.892
N210G1X32.025
N220G1Y32.108
N230G1X11.705Y11.788
N240G1X134.345
N250G1Y623.211
N260G1X11.705
N270G1Y11.788
N280G00Z5.080
N290G00Z20.320
N300M05
N310M30
%

[Rcnewcomb]

From another thread

can somebody point me to a reference to understand the code in the mmg file?

Wikipedia has a write-up on understanding ->G code.

A few of the critical commands:

G0 = Rapid Position
Example: G00 X7 Y8 Z1
Does a rapid move from the current position to XYZ position 7,8,1. All three axes move at the same time.

G1 = Move
Example: G00 X7 Y8 Z1
Moves at the feed rate from the current position to XYZ position 7,8,1. All three axes move at the same time.

F = Feed rate - units are distance per time. Could be inches per second, Inches per minute, meters per minute, etc. The units are defined by the controller software. it can be on a separate line or included with a move command
Example: G1 X8.75 F60
Moves from the current position to X 8.75 at a feed rate of 60 (probably inches per minute)

S = Spindle Speed (usually RPMs)
Example: S12000
Sets the spindle speed to 12,000 RPM.

M = Machine command
Examples: M03 = spindle on, M05 = spindle off

Some controllers have line numbers included in the G code. The following code was generated using the Axiom Metric post processor, so units are in millimeters.

Looking at the first 10 lines of the file:

(Filename: VcarvePocket 1)
N10M03S12000
(Pocket 1)
N30G00X57.199Y58.275Z5.080
N40G1Z0.000F762.0
N50G1X82.599Z-0.635
N60G1X57.199Z-1.270
N70G1X88.851F2032.0
N80G1Y576.725
N90G1X57.199

The first line is just a comment with the file name.
(Filename: VcarvePocket 1)

The next line has a line number, a command to turn on the spindle, and the speed of the spindle
N10 M03 S12000

Line N30 does a rapid move to the position specified by the X, Y, and Z coordinates, These are in millimeters because I used a metric post processor.
N30 G00 X57.199 Y58.275 Z5.080

Line N40 moves the Z to 0 and sets the feed rate to 762 millimeters per minute (about 31 inches per minute)
N40 G1 Z0.000 F762.0

Line N50 moves at the feed rate to X82.599 (it was at X57.199) and at the same time moves the Z down to -0.635 mm (-0.025")
N50 G1 X82.599 Z-0.635

Line N60 moves at the feed rate back to X57.199 and further ramps the Z down to -1.27mm (-0.05")
N60 G1 X57.199 Z-1.270

Line N70 moves to X88.851 mm with a new feed rate of 2032 mm/min (80 IPM). The Z remains at -1.27mm
N70 G1 X88.851 F2032.0

Line N80 now moves at feed rate in the Y direction to Y576.725
N80 G1 Y576.725

Line N90 moves at feed rate in the X direction back to X57.199
N90 G1 X57.199

[tunacnc]

I looked at both files. They are not identical, so the G-code generated is slightly different between the two.

Thanks for checking it and validating what I am seeing. I originally just dragged the X and Y free hand, so yes they are different. I remade the files and specified that the offset it .5" all the way around the material they should be identical now. The gcode for the z axis seems to be identical but the X and Y toolpaths are different. I removed the ramp for simplicity.

Thanks for help, I'm learning alot. I'm new to gCode, so had to do some googling to figure out what the commands were.

I'm gonna test run these new files and see what happens this time.

Code: Select all

(Filename:  V1Walnut)
N10M03S12000
(Pocket 1)
N30G00X59.436Y59.436Z5.080
N40G1Z-1.270F762.0
N50G1X86.614F2032.0
N60G1Y575.564
N70G1X59.436
N80G1Y59.436
N90G1X36.068Y36.068
N100G1X109.982
N110G1Y598.932
N120G1X36.068
N130G1Y36.068
N140G1X12.700Y12.700
N150G1X133.350
N160G1Y622.300
N170G1X12.700
N180G1Y12.700
N190G00Z5.080
N200G00Z20.320
N210M05
N220M30
%

Code: Select all

(Filename:  a1Walnut)
N10M03S12000
(Pocket 1)
N30G00X53.340Y53.340Z5.080
N40G1Z-1.270F762.0
N50G1X92.710F2032.0
N60G1Y581.660
N70G1X53.340
N80G1Y53.340
N90G1X33.020Y33.020
N100G1X113.030
N110G1Y601.980
N120G1X33.020
N130G1X33.020Y33.020
N140G1X12.700Y12.700
N150G1X133.350
N160G1Y622.300
N170G1X12.700
N180G1Y12.700
N190G00Z5.080
N200G00Z20.320
N210M05
N220M30
%

[tunacnc]

Thanks for posting the GCode command definitions. I spent the past hour scratching my head trying to figure it out.

[Rcnewcomb]

Thanks for posting the GCode command definitions. I spent the past hour scratching my head trying to figure it out.

Each person here started at the beginning. The help I received from others when I got into this 15 years ago was critical for my ability to get the infernal machine to do anything useful.

Once you get a repeatable process that ends in success you will be amazed at what you can get the machine to do for you.

[tunacnc]

The new file seems to be working now. Thanks for the help. I'm still unsure why it was behaving that way right after I upgraded, so I'm gonna fly cut a couple of my future carves before I trust it again.