DeskProto user forum

I'm new to DeskProto, but not to CNC. Have made many itme, so I know my hardware and MACH4 are working fine.

I'm trying to make a small 25X50mm chess piece (Knight). I'm using the setup exactly as the Venus example. Strategy Parallel, reverse X axis. Ramp angle 3 degr Skin 1mm. Protect Vertical Surfaces is checked.

It works fine knocking off the corners of the material and then it starts digging a ditch. I have the layer Height set to 2mm (Custom) in the Roughing tab. Z moves down 2mm at a time, but after going down 6mm in this ditch (2mm at at time) it rotates the A axis and starts makein a 6mm deep cut until I stop everything. I'm watching the DRO display and Z drops from 16 to 14 to 12 as it digs this ditch. At Z12, it is down 6mm from the rest of the part. I've tried may different settings, but same result everytime.

Hope someone can help me with this. Here's a picture of the 6mm cut.

Are you regenerating the toolpaths after making adjustments?

... And resaving the new gcode?

yes, I'm now trying with "Sort" unchecked. will update if this works or not.

Turning off Sort did not fix the Problem.

After the corners are knocked off the material, It is still plowing a 6m deep ditch the full lenght of the X axis, going down 2mm at a time. It then moves about 5mm down the ditch and executes an A360 gcode. This attempts to cut a 6mm deep band around the work piece, before I hit stop.

Giving up for today.

For rotary problems with Mach3 it is good to first check FAQ issue faq.php#problems4.
I do not know though if this is also true for Mach4, and it also does not explain the ditch along X.
Are these error paths visible on the screen ?
Feel free to send me a Problem report zip file (can be made in the DeskProto Help menu) for this project, send it to info at deskproto dot com.

Lex, thank you, report sent.

The cut around the A Axis up about 5mm from the bottom is where I stopped it, as it was about to pull the part out of the chuck.

Do these cuts show up as part of the toolpath in DeskProto?

A screen-shot would be interesting to see.

Hi DB and Blowlamp,

I had reacted on the problem report file by email.
Will repeat my reaction on the forum, hoping for more innput, for instance from other Mach4 users.

----------
Thanks for sending this problem report file, now I could reproduce the situation.
I calculated the NC file and ran in in my G-code previewer, and the results seemed fine.

So I looked into the G-Code, and where Z16 starts I found these lines:

G1 Z16.042 F750
G93
G1 A360.000 F6.6
G94
G1 X58.223 F750
G93
G1 A0.000 F8.8
G94
G1 X57.334 F750
G93
G1 A360.000 F8.8

So the cutter needs to rotate from A=0 to A=360, make one step along X, then rotate back to A=0, etc, until X= 0 is reached. Then the cutter moves to Z14 and a similar series of commands follows.

My theory is that your machine simply 'thinks' that A=0 equals A=360 and therefore does not rotate. The result will be one long ditch along X.

Have you checked the FAQ issue that I mentioned on the forum ? That is exactly about this problem.

The G93 commands tells the machine to use "inverse time feedrate". Does Mach4 indeed support that ?

A possible workaround is to keep the machine rotating in the same direction, so from A=0 to A=360 to A=720, etc. No idea if that will solve this, it may be worth a try.
A second workaround can be to select parallel toolpaths Along X instead of Around A.

Still it will of course be best to detect why this goes wrong,