[spelunker]

I've got my Series II, Boss 6 finally up and running somewhat reliably in my garage now... so I have a question on the syntax for using polar coordinates. The programming documentation I've acquired is for an earlier control and doesn't cover this feature. What I am attempting to understand is the use of G03 circular interpolation while providing (A)ngle and (R)adius parameters. I am also confused with I and J being specified as absolute coordinates for the arc's center. Can a Z axis move be incorporated with a G03 move? Could anyone shed some light on this for me... it would be greatly appreciated!

- Tim
(scratching head!)

[machintek]

Iy boots into G17 which is X & Y G02/3. If you specify G18 or G19, it becomes X and Z or Y and Z.
Either use I J (signed incremental value from start point to circle/arc center, OR use the X, Y and R. I never bothered to use the A.
To do simultaneous X Y AND Z is considered helical and I am not sure the BOSS 6 does it. Consult the programming manual.

George

[spelunker]

Thank you for your answers George. I believe I was somewhat unclear in my original question. My programming manual is for a pre-Boss 5 control that didn't even support multi-quadrant circular interpolation much less (A)ngle and (R)adius syntax.

I've attached a couple of pages from a Bridgeport comparison document that briefly describes the updated features of Polar coordinates in the Boss 5-6 controls. It states the possibility of cutting a radius vector distance for a given angle. Also the ability of a helix by utilizing looping.

My attempts at using X, Y, and (R)adius in cutting arcs in the XY plane have been troublesome since it is unclear how the center of the arc is specified (I and J?, incremental or absolute? G91, G90). The attached PDF seems to indicate G75 can be used with I and J specified as either absolute or incremental. The G-Code tests that I've done on the mill do not seem to operate as I would have guessed.

Do you know of any documentation available for this? I'm really curious as to the ability of cutting arcs in the XY plane that include an increasing Z depth.

Thanks for the help.
- Tim
See attachment...

[Kevin Taylor]

I had a hard time understanding this on my boss 7.2 sounds like you could have the same problem I had I found it best to give a G75G90 in the last G0 or G1 before the G3or G2 Then your I&J are the abslute point of arc center fromX0Y0 easy to rember rather than start point to arc center +-Xor Y for the I&J respectivly Practice in air,wood,wax or plastic it break's less tooling I have yet to manage to spirle I dont think it will do multi qud with Z If you are self taught CNC like me every time you run it you learn a new trick Kevin

[lakeside]

Your controller is using stander EIA format G, M, code info is very easy to find on web and the best trick to save on broken tools is to run path before loading tool

[spelunker]

Here is a sample listing that does not run on my Boss 6 control as I would expect. It is a simple spiraling circle pocket that concludes with a 2.6 inch radius tool path:

N10 G90 G75 G17
N20 G00 X0.0 Y0.0 M06 T1
N30 G00 X0.0 Y0.0 Z0.100
N40 G01 Z-0.005 F100
N50 G3 Y0 X0.35 R0.175
N60 Y0 X-0.35 R0.35
N70 Y0 X0.7 R0.525
N80 Y0 X-0.7 R0.7
N90 Y0 X1.05 R0.875
N100 Y0 X-1.05 R1.05
N110 Y0 X1.4 R1.225
N120 Y0 X-1.4 R1.4
N130 Y0 X1.75 R1.575
N140 Y0 X-1.75 R1.75
N150 Y0 X2.1 R1.925
N160 Y0 X-2.1 R2.1
N170 Y0 X2.3 R2.2
N180 Y0 X-2.3 R2.3
N190 X2.3 Y0 R2.3
N200 Y1.4922 X0.8077 R1.4922
N210 G00 Z0.1
N220 M02

I have simulated this code using Mach3 and it appears to run fine.

Thanks for all the suggestions thus far... I haven't destroyed any tooling since I test these programs with my tool TLO set way above the material until I sense the movements are correct.

Does anyone have a Boss 5 or 6 program manual that might explain the proper syntax?

I find it somewhat humorous that when the Bridgeport interpreter decodes a line of code it doesn't understand, it seems to move the axis motors in weird ways... instead of raising an error on the control panel.

Thanks.
- Tim

[lakeside]

your code does look good here the veiw from metal cut

[spelunker]

I think this might have something to do with the subtle differences in how the R is interpreted. I was reading here:
http://www.nfrpartners.com/nfrg2g3.htm

...and it mentions the R syntax can infer two arc centers. Using + or - might choose an arc < 180 or > 180 degrees. This might be cleared up in the Boss 5/6 programming manual.

Thanks.
- Tim

[lakeside]

you may also be able to program using I and J heres a sample program for a 4" pocket dia. circle using a 1/2 cutter path you need add you program start and G90 to start line and add end info. edit Z hights

[Kevin Taylor]

The boss 6 is going to use I&J for the radis A 2" arc tool path at X2.0Y2.0Arc center would be
G0G90X0.0Y0.0
G75G90
G00Z0.0S500M3
G00X0.0Y2.0M8
G01Z-.100F50
G03X0.0Y2.0I2.0J2.0
G01Z-.200
G03X0.0Y2.0I2.0J2.0
G01Z-.300
and so on I dont think you can do Z unless it is one quarter at a time not in multi Qudrant The G75G90 makes the arc center the same as I&J G75multiQud G90Abslute
Watch Ebay for manuals Good Luck Kevin

[spelunker]

I've decided to use the absolute G03 with I and J syntax until I can find further documentation. It's unfortunate that there are so many flavors of G-code for the various controls.

I am writing some simple G-code generating wizards and wanted to stay somewhat compatible with Mach3. It doesn't look like that will be particularly feasible from what I can decipher at the moment.

Thanks for everyone's input! I'm now on the prowl for a Boss 5/6 programming manual...

- Tim

[lakeside]

Attached Your Will Find A File For A 2" Arc Only 180 Degs. Arc Center Is X2. Y2. Z Goes From .5 To 0.0 This Is A 3d Path You Can Try It To See If Your Contoller Will Do An X, Y, Z Circle Intrepulation

[spelunker]

lakeside -

Thanks for the file. I can see from the code that my controller will have no problem running this... it is simply 3D straight line vectors (G01). I have generated these myself from a helical wizard I was working on... one drawback to this is the fact that it takes so many lines of code to define a smooth path. My Bridgeport has a somewhat small program memory and these files can be huge. I suppose one of my next projects could be a "drip feed" of some type - I think I know a scheme that might work.

Everything is much appreciated!
- Tim

[lakeside]

Do You Have An Rs-232 On Your Controller?

[spelunker]

RS-232 yes indeed... though it's not the fastest. I believe I'm running 4800 baud.

[lakeside]

So Can YOU Run Dnc For Very Long Programs To Controllers Buffer

[spelunker]

I suppose I can run DNC to the Bridgeport's controller but I don't have software to do that at the moment. Like you mentioned... I could run large programs that won't fit in the controller's program buffer if I did.

[lakeside]

Dnc Software Is Cheap There Are Many Companies That Have It

[machintek]

The BOSS 5 will not support DNC unless you have the Bridgeport DNC loader. I know that now BTR (behind the tape reader) units are sold but do not know of anyone running one.

BTW, I had one person trying to make a cam profile and it was coming out wrong. He was using R instead of I J. I admit that the R is easier but a radius can fit between two point in more than one way. When he switched to I J, the cam came out correct as the radius center was specified.

George

[spelunker]

I am now set on using I and J for G02, G03 commands. Unfortunately absolute I and J coordinates are not compatible with Mach3 which I was using to simulate my tool path for testing.
The operating manual I have mentions that sending the "escape" character to the machine while in edit mode will cause the machine to execute the current line in the buffer. I might test this sometime to see if it would be feasible to create an application on Windoze that would feed the machine a line, execute it, delete it, and then repeat the process for a complete file... it might behave like a crude DNC. There may be some problems with this in practice.

- Tim