DeskProto user forum

Hi, I have a question that I could not find an answer to in the forum. I would be very grateful if anyone could help me.

When I have created a file for my milling machine and start the job, the tool moves to the workpiece zero point (the point I set as zero in DeskProto and then also in the milling machine so that both match), and then continues to the point where it should begin milling. The tool goes to the zero point in the X and Y directions, but not quite in Z – instead, it stays a few millimeters above the zero point.

The problem is that I often clamp the workpiece at the zero point, so when the tool moves there it risks colliding with the clamp I use to secure the workpiece. Since the tool moves to the zero point but stays a few millimeters above it in Z, it should be possible to set the height it keeps during this movement, right?

I can set the height to (for example) 30 mm at "Free movement height" in the Z settings tab but before going to to 30 mm, the tool goes to the zero a couple of millimeters above the workpiece.

Could it be a tool offset problem?

Martin.

That is strange: DeskProto does not start the toolpath with a movement to the workpiece zero point. You can check that by viewing the NC file in a text editor.
Can it be that your control software somehow adds that movement ?

@Lex: That's not 100% correct. :)
In the default job parameters, this can be set under “Extra NC commands” and will then apply to every new job.
Of course, it is not active by default and must be activated separately.

Hi MaFu, Your are of course right. Though I do not expect that after setting this (rather hidden) command a user would completely forget about it...
Lex.

Hi and thank you for your answers, I really appreciate it! First I did like MoFu suggested and checked the default the "exta NC commands" under under "default job parameters" but there were no changes from default. Then I checked the NC file and the beginning of the file looks like this:

G00 X0 Y0 Z10 F120
M10 O2.1
G00 X103.717 Y76.746 Z10.000
G01 X103.717 Y76.746 Z0.000 F60
G01 X103.655 Y76.673 Z-0.008

I am absolutely no guru at understanding NC commands but the first line seems to be the one that moves the tool to 10 mm above the zero. I assume that I can change the value 10 to, for example, 60 to solve the problem?

//Paul

Hi Paul,

That surely is strange.
The only other place that I can think of is the postprocessor: this first line could be one of the Start commands that have been set in the postprocessor that you use. You can find these via
Options > Library of postprocessors > OK on warning > Select your postprocessor and press Edit > tab Start/End.

If that does not help then please create a 'Problem report' zip file for your project (can be done in the Help menu) and email that to us.

Lex.

Hi again Lex,

You are right, I found the error in the post processor. I am using the one named "Kosy CNC machine" and the default setting under Start/End is:

rem: NC program file
rem: from DeskProto for Kosy machine
G00 X0 Y0 Z10 F120
M10 O6.1

I am grateful for the help and suggestions from you all, thanks! :)