This is tortuous

[Robin Hewitt]

Still trying to figure out how to interpret these G codes from G-Simple.

In the picture are 3 consecutive G03 arcs, the yellow lines show the tool path.

If I read it right...

N1229 spirals down in to the round bearing cutout at the bottom giving a smooth entry to the cut.
(His animation doesn't show the z shift so the lines don't join up).
N1230 finishes the face.
N1231 is a smooth exit back to center.

Without the EIA definition for RS247D g codes, this suggests that x,y and z stay the same if omitted, while I### overrides a previous R###.

I'll have to rewrite my arc cutting routine to include a shift in z. I'm nearly there but it ain't easy

[ger21]

Looks like:
1228 - plunges down to Z-17.5
1229 - ramps down while doing a 1/2 circle to Z-25.4 from the center of the hole
1230 - does complete circle.
1231 - half circle back to center of hole
1232 - retract tool to Z 10

[ger21]

Originally Posted by Robin Hewitt this suggests that x,y and z stay the same if omitted, while I### overrides a previous R###.

Yes, correct.

No idea why he's mixing R arcs with IJ arcs, although it appears that he's using IJ to do full circles. I prefer to use IJ only.

[Robin Hewitt]

Originally Posted by ger21 Yes, correct.

Code re-written

G-Simple looks to be okay. The only bit I found really annoying was that the materials a tool can cut are defined by name, eg: carbon steel, but the material you are cutting is defined by number, eg: ST-14 which means zip nada to me. It would be nice if I could substitute EN numbers or just escape having to match tool to material altogether and set my own feed rates, but at this price I can't complain.

Couple more days work and I should have it cutting metal.

Thanks for the help, I was thinking his I### indicated a 360 degree cut, rather than when x, y (and possibly z) stay the same. Seems to be working now, I've put in a squeaker that will go off if it ever finds a J###.

Sure is easier to locate the arc center with that I###

[S.Kontogiannis]

A note about GSimple and materials:

There is a file in GSimple called material.dat. It is an ascii (plain text) file. You can edit it with notepad or any other text editor. This is the file that assosiates Material Names with the Material Gropus/Subgroups. For example the line about CK45 reads:

CK45 1.3

indicating that CK45 belongs to group/subgroup 1.3

You can edit this file, and make it as you wish. For example you could just write:

Group_1.1 1.1
Group_1.2 1.2 etc

The only material you should not delete is ST37-2 (this is the default material).

By the way, Groups and Subgroups are alse not fixed. They are defined in the file amg.dat (also a plain text file). You can change them too, if you like.

[ger21]

Originally Posted by Robin Hewitt Thanks for the help, I was thinking his I### indicated a 360 degree cut, rather than when x, y (and possibly z) stay the same. Seems to be working now, I've put in a squeaker that will go off if it ever finds a J###. Sure is easier to locate the arc center with that I###

You need the J as well, unless it hasn't changed from the previous move, which was the case in your example.

I = the X coordinate of the center
J = the Y coordinate of the center

They can be either absolute postions, or relative to the tool position at the start of the arc, which is what you're example used I believe.

[fizzissist]

Don't know if this will help or just slow things down...and I don't know if the difference between the RS247D and RS274N standards is program/computer/controller problem for your system....but here is a couple of links anyway!

http://www.isd.mel.nist.gov/personne...4NGC_3TOC.html

http://www.linuxcnc.org/handbook/gcode/g-code.html

Me? I prefer using I and J, since I know (at least on my controllers) that since they're incremental from the start point, I can easily find the center, or know where the center is supposed to be.

[Robin Hewitt]

Originally Posted by S.Kontogiannis A note about GSimple

Thanks for that and thanks for the software

I'll do the materials later, today I'm writing the tool locator...

Question: I want to convert the g-codes to robin format and tack in the original shape from the dxf (makes for more interesting graphics). Can I replace the CopyTo program with my own?

I tried...

TRANSFER "c:\Program Files\Gsimple\CopyTo a g.cnc"

and got an error...

Usage: CopyTo <drive> <file>

In reply to Ger21...

Can't do J unless it throws one up so I know which way to leap

Obviously I still have a lot to learn. Think I'll start by cutting MDF rather than metal for the testing.

best regards

Robin

[S.Kontogiannis]

Question: I want to convert the g-codes to robin format and tack in the original shape from the dxf (makes for more interesting graphics). Can I replace the CopyTo program with my own?

Answer: Yes, you can. Just replace the CopyTo.exe reference in the configuration file with a reference to your program. For example, lets say you make a program which transfers the code via RS232 to the milling machine and the program is called MyTransfer.exe. The program must be able to get the filename to be transfered as argument.

From the dos prompt you would type

c:> MyTransfer g.cnc

and MyTransfer would transfer the file g.cnc to the milling machine

The line

TRANSFER "c:\MyTransfer"

in the configuration file will do just that. Whenever you press the transfer button ot will call MyTransfer.exe with argument the gcode file.

[Robin Hewitt]

Hi SK

I nearly tried it out today, sadly the PC next to the mill overdosing on oil, swarf and soot turned it's toes up.

I was given a PC recovered from a skip but it didn't have the speed. All the movements were there and it did the straight lines okay, but couldn't hack 1024x768 graphics and cut curves at the same time. The steppers became very jittery and unhappy when driving 2 axes.

I'll disable the part that draws the cutter and try again tomorrow

best regards

Robin