G-Code outside circle Heidenhain

[bigtoad170]

I have a bridgeport series II interact II heidenhain tnc151a programming g-code in inches I'm trying to make a 2 inch diameter boss .750 deep in aluminum 6061 I 've been able to do it but I had to go and edit the z depth everytime I got the job done but for the next time around I need to know a more efficient way I'll show you how I've been doing it. The center of the boss is the origin. Cutter radius .313

N10 G00 G90 Y0 X-1.313 z+.1
n20 G01 z-.1 F100
N30 G90 I0 J0 G12 H-180 F200

I let it run go edit the -z and let it run etc...
Take it easy on me I'm a newbie on programming and this is all I could do to get it to work I wanted to set up a label and have a G91 for the -z so everytime it looped around it would increment down a .100 at a time I had no luck at that says I was missing a tool call

[kdhBOSS5VRAM]

I drew out what you were doing and posted it with what I think is a G code Heidenhain post. I never use it in G code. I always use it in plain language programming. With that you could do it in a few lines with a helix. (2nd example). I don't know how you do the helix in G code. I'd have to check. You could do what you are doing with a label also but the helix is easy as long as you have the right end mill and material. It's constant motion in all 3 axis. Hope this helps.

Kevin

%UNTITLED G70
N2 G01 G40 G91 Z0,0 F6000 M91
N3 G99 T1 L0,0 R0,0
N4 T1 G17 S2000
N5 G01 G40 G90 X-5,0 Y5,0 M06
N6 G01 X1,313 Y0,0 M3
N7 G01 Z0,1 F6000 M
N8 G01 Z-0,1 F100
N9 G90 I0,0 J0,0
N10 G02 F200
N11 G01 Z-0,2 F100
N12 G90 I0,0 J0,0
N13 G02 F200
N14 G01 Z-0,3 F100
N15 G90 I0,0 J0,0
N16 G02 F200
N17 G01 Z-0,4 F100
N18 G90 I0,0 J0,0
N19 G02 F200
N20 G01 Z-0,5 F100
N21 G90 I0,0 J0,0
N22 G02 F200
N23 G01 Z-0,6 F100
N24 G90 I0,0 J0,0
N25 G02 F200
N26 G01 Z-0,7 F100
N27 G90 I0,0 J0,0
N28 G02 F200
N29 G01 Z-0,75 F100
N30 G90 I0,0 J0,0
N31 G02 F200
N32 G01 G91 Z0 R0 F6000 M91
N33 G01 G40 G90 X-5,0 Y5,0 M05
N34 G01 G40 G90 F6000 M02
N9999 %UNTITLED G70


1 BEGIN PGM HELIX INCH
2 L Z0 R0 F3999 M91
3 TOOL DEF 1 L0 R0.0
4 TOOL CALL 1 Z S2000
5 L X-5.0 Y.0 R0 F3999 M6
6 L X1.313 Y0.0 R F M3
7 L R F M
8 L Z0.1 R F3999 M
9 L Z0 R F100 M
10 CC X0.0 Y0.0
11 CP IPA 2880 IZ-.750 DR- F200 M
12 L Z0 R0 F3999 M91
13 L X-5.0 Y0 R F M91
14 L R F M2
15 END PGM HELIX INCH

[bigtoad170]

Hey Kevin Wow thanks alot man you took alot of time to help a guy out I'm not at my machine right at this moment but I'll give it a shot thanks again I'll keep you posted on the progress

[kdhBOSS5VRAM]

I looked in the ISO programming book (G Code) on how to do a helix and it looks like if you modify what you were using slightly you could do it that way. Try it and see what happens.

N10 G00 G90 Y0 X-1.313 Z+.1
N20 G01 Z0 F100
N30 I0 J0
N40 G12 G91 H-2880 Z-.75 F200

The H number is 2880 degrees which is 8 revolutions down .750 so a little less than .100 per rev. I'm not sure of the + or- on the H. I think that will control the direction it spirals. Of course you'd want to have another line after with a G90 G00 to bring Z back up. I did try what I gave you before for the conversational program modified for a TNC430 control and it did work fine.

Kevin

[bigtoad170]

Kevin thanks that was the ticket worked great much more efficient thanks for your time on figuring that out for me

[troy.edwards]

Just a question, why are you programming in the ISO format. Heidenhein is a superb language & i have been working with it for 18 years now (from basic work to 3D forms) i have also had alot of dealings with fanuc & acramatic 2100 & I will say that hands down heidenhein will blow the others away by far for ease of use + flexibility. I can give you a solution in heidenhain which would use parameter programming (it's sounds fancy but it works well & easy to understand) or if you like you could use incremental moves & a lable repeat if that would be better.

Troy.

troy.edwards@talktalk.net

[marsmach]

Hi I,m with Troy on this Heidehan far simpler language,using variables and label repeats far easier regards G

[bigtoad170]

I guess I just wanted to know what seems to be the universal language first g-code. It has been going well and actually it was worth it because unfortunately one of the cnc programmers at my 9-5 job had a stroke and I was able to have a easy transition to take his jobs over since he programs in g-code that way they didn't have to hire someone to take his position while he recovers and will have a job when he comes back.