Programming Advice

[Bill OConnell]

I am a little rusty at programming and I would like to run a few things by the forum before I drive a bit through the table.

I am trying to make two oval blocks with a profile out of soft maple. I will test this on MDF first, but I would like some validation of my set up.

After placing my material on the table I will locate the corner closest to home and enter the coordinates into the fixture table (F4,F4) so that I can use a G52 command. The X and Y coordinates to use are pretty straightforward, but I am not sure about the Z. Should that be the surface of our spoilboard? If so, can I use the Daylight value of the currently loaded tool for that and just verify it?

If my assumptions are so far correct, my new 0,0,0 (absolute) location will be the corner of my material closest to machine home and on the spoilboard surface, correct? Now any positive ZSHIFT values will lift the Z zero value (absolute) that amount, so if I want to test the pattern I can set ZSHIFT to, say, 3\".

If I am satisfied with the pattern and I let ZSHIFT equal the thickness of my material plus any wasteboard, my Z zero coordinate should be at the surface of the material I want to cut. I can then position the router head a safe distance above the part for travel purposes by moving the head to, say
G01 Z1
which would place it 1\" above the material. At that point I could switch to incremental mode and cut my pieces plunging 1\"+ my desired depth of cut and then retracting the same amount.

After cutting this piece if I go back to Absolute mode, would that again put 0,0,0 at the corner of the piece closest to machine home on the surface of my spoilboard? If I then wanted to cut the second piece, using by copying the same code, I would just have to relocate the origin either through a new entry in the fixture table or by moving the head to, say, 10,0,0 (absolute) and using a G92 code, correct?

I know this is rather long winded, and I appreciate your patience, but we are still new at this and we don't have the depth of self confidence to go this route without the great help from this forum.

[Jody Wilmes]

\"I am a little rusty at programming and I would like to run a few things by the forum before I drive a bit through the table.

I am trying to make two oval blocks with a profile out of soft maple. I will test this on MDF first, but I would like some validation of my set up.

After placing my material on the table I will locate the corner closest to home and enter the coordinates into the fixture table (F4,F4) so that I can use a G52 command. The X and Y coordinates to use are pretty straightforward, but I am not sure about the Z. Should that be the surface of our spoilboard? If so, can I use the Daylight value of the currently loaded tool for that and just verify it?\"

Do not put anything in for the Z value...not even zero, just leave it blank. Your daylight value will take care of this offset. The only time you need to worry about the Z value in the fixture offset table is if are running a 5-axis program.

\"If my assumptions are so far correct, my new 0,0,0 (absolute) location will be the corner of my material closest to machine home and on the spoilboard surface, correct? Now any positive ZSHIFT values will lift the Z zero value (absolute) that amount, so if I want to test the pattern I can set ZSHIFT to, say, 3\".\"

As stated before, the absolute position for X & Y will be the corner of material closest to Home. The tool's daylight value is the absolute position from Home to the spoilboard surface. At the point the G52 is called, your X0Y0 is set. At the point the tool# is called, your Z0 is set.
You are correct about the ZSHIFT value.

\"If I am satisfied with the pattern and I let ZSHIFT equal the thickness of my material plus any wasteboard, my Z zero coordinate should be at the surface of the material I want to cut. I can then position the router head a safe distance above the part for travel purposes by moving the head to, say
G01 Z1
which would place it 1\" above the material. At that point I could switch to incremental mode and cut my pieces plunging 1\"+ my desired depth of cut and then retracting the same amount.\"

Correct. An alternative is to keep the entire program in absolute mode. This way your Z values are based off the ZSHIFT (material surface) and not the last postition. This is extremely helpful if thickness changes. It may take a little bit to get used to, but worth it.

\"After cutting this piece if I go back to Absolute mode, would that again put 0,0,0 at the corner of the piece closest to machine home on the surface of my spoilboard?\"

Yes it would.

\"If I then wanted to cut the second piece, using by copying the same code, I would just have to relocate the origin either through a new entry in the fixture table or by moving the head to, say, 10,0,0 (absolute) and using a G92 code, correct?\"

Correct. You would only need to G92 X0 Y0. No need to do the Z (daylight value)

\"I know this is rather long winded, and I appreciate your patience, but we are still new at this and we don't have the depth of self confidence to go this route without the great help from this forum.\"

Seems like you got it with the exception of the Z value in the Fixture Offset Table (leave blank). A VERY valuable piece of code you can add to the beginning of your program is M48 and M49 at the end of the program. This allows you to use the FeedRate OverRide Knob on rapid movements, etc. Thereby reducing the chances of a \"crash.\" Once your program has been proofed and you're satisfied, remove the 2 codes and the machine will run faster and more efficient. Oh and save it!

[Bill OConnell]

Jody,

Thanks a million. I feel a lot more confident as I approach this program.

Regards,
Bill