Tools float above workpiece

[adrewfis1980]

Now that the mill hardware works correctly and have uploaded 1st post process from Fusion 360 to the CNC12 software, I've run the program several times and each attempt I get, each of the tools float above the workpiece about 1-2 inches and never engage the part. It appears to have the correct tool paths shown in Fusion 360 but the Z depth is obviously not correct. I have set all the associated tools for this program to correct offsets and have set all the axis to zero correctly. I'll post the process here for reference. Thanks for your help!

Titan 1M - New Op1.nc

(258.34 KiB) Downloaded 1 time

[cncsnw]

While it is running, and the tools are not at the depth you expect, you need to look at four things:
1) What are the Z coordinates called out in the G codes. In the program you posted, the facing is at Z0.0, and the next operation is down around Z-.760, so that is probably correct.
2) What Z coordinates are shown on the DRO display as it runs?
3) What is the active H offset number, shown in the status window display?
4) What is the current work coordinate system (WCS) in the top left corner above the DRO?

If you are used to only looking at the Runtime Graph display -- as many Acorn users are -- you should get in the habit of also looking at the normal G code display as the job runs. Press F8 to switch back and forth. There is a lot of useful information on the G code display, including the complete status window; multi-line message box; more legible DRO; and more lines of your CNC program before and after the current line, to provide context.

If all your tools cut too high by the same amount, and the Z position on the DRO says they are all cutting at their correct depths, then it is probably an error in setting the Z axis Part Zero location.

It is also possible that you set your Part Zero in some coordinate system other than G54 (WCS #1); but since your CNC program calls out G54 at the start of every operation, it is going to run in G54 regardless of what you had selected when you set your Part Zero.

[adrewfis1980]

While it is running, and the tools are not at the depth you expect, you need to look at four things:
1) What are the Z coordinates called out in the G codes. In the program you posted, the facing is at Z0.0, and the next operation is down around Z-.760, so that is probably correct.
2) What Z coordinates are shown on the DRO display as it runs?
3) What is the active H offset number, shown in the status window display?
4) What is the current work coordinate system (WCS) in the top left corner above the DRO?

If you are used to only looking at the Runtime Graph display -- as many Acorn users are -- you should get in the habit of also looking at the normal G code display as the job runs. Press F8 to switch back and forth. There is a lot of useful information on the G code display, including the complete status window; multi-line message box; more legible DRO; and more lines of your CNC program before and after the current line, to provide context.

If all your tools cut too high by the same amount, and the Z position on the DRO says they are all cutting at their correct depths, then it is probably an error in setting the Z axis Part Zero location.

It is also possible that you set your Part Zero in some coordinate system other than G54 (WCS #1); but since your CNC program calls out G54 at the start of every operation, it is going to run in G54 regardless of what you had selected when you set your Part Zero.

Thanks for the reply.

1). The Z coordinates called out in the G codes are correct for the part.
2.) The Z coordinates shown on the CNC12 DRO are correct for each operation of the part.
3). My tools/offsets in CNC12 did not match the T numbers from the program in Fusion 360 so I changed them to reflect the same tools. I set the 1st tool Face Mill to zero on the part and offset the rest of the tools #'s 2-5 based on that height. This caused the tools to be even higher off the part than before. Do these tool numbers in CNC12 need to match the tool #'s from Fusion? I had these set up differently (did not match Fusion tool numbers) and they were closer to the part but still about 1-1.5" away from where they needed to be.
4.) The current work coordinate system in the upper left corner is WCS #1 for both running the part and when I zero'd all the axis.

See below for videos of what's going on. The face mill is the worst offender at roughly 1.5200" above the surface. This part was added in Fusion with the dimensions from the part and the rest of the tools were from a tool library I had downloaded and purchased those tools. The rest of the tools seem to be 1" above. As stated above I have zero'd all the tools in WCS #1 and ran the part program in the same WCS.

https://www.dropbox.com/scl/fo/95grkb6m ... gg30y&dl=0

[suntravel]

Related reading:

https://www.centroidcnc.com/centroid_di ... rement.pdf

Uwe

[Houseman303]

create a tool table in Fusion, it must match the tool table in CNC12. The values ​​in Fusion are for simulating and calculating tool paths. The D and H values ​​in CNC12 are the values ​​used for machining. D only for radius compensation, H always.

[adrewfis1980]

Thanks guys, it seems both suggestions took care of the problem. Setting parameter #3 to 4 and making a library in Fusion 360 that matched the one I have on CNC12. Thanks again!

[suntravel]

With CHIPS you can import fusion tool tables in CNC12

Uwe

[grossmsj]

With CHIPS you can import fusion tool tables in CNC12

The first hour CHIPS comes out with ATC support, I'm on it. It looks like an incredible addition to CNC12.
I love the ProbeApp, and just don't want to let go of how easy the ATC works in it.