Could use some Help. Programming (I think)

wellman91 · Feb 3, 2020

Could use some help. Im running a part that every operation works but my corner round (contour) and a boring cycle. I have triple measured the tool length offset and I have deleted the tool in my CAM software assigned it a new tool number, remeasured the tool length and it still doesn't work. Those two operations end up 2 inches above the part. all the other operations end up perfect. attached is the boring cycle. Im sure its right in front of me but I'm not seeing it. I use Fusion 360 CAM and have never had anything like this. Thanks for any help.

I have a Leadwell V-20 2004 With an OIMB Fanuc control.

O1002 (INTEGERAL LINK)
(T15 D=1.1875 CR=0. - ZMIN=-0.77 - BORING BAR)
G90 G94 G17 G49 G40 G80
G20
G28 G91 Z0.
G90
(DRILL1)
T15 M06
S1000 M03
G54
M08
G00 X0.8295 Y-0.875
G43 Z0.6 H15
G00 Z0.2
G98 G85 X0.8295 Y-0.875 Z-0.77 R-0.065 F5.
X7.1705
G80
Z0.6
M09
G28 G91 Z0.
G90
G49
G28 G91 X0. Y0.
G90
M30
%

g-coder05 · Feb 3, 2020

Aside from too much wasted code it looks ok. Are you sure your tool lengths are set right?

O1002 (INTEGERAL LINK)
(T15 D=1.1875 CR=0. - ZMIN=-0.77 - BORING BAR)
G90 G94 G17 G49 G40 G80 G20
(DRILL1)
T15 M06
S1000 M03
G00 G54 X0.8295 Y-0.875
G43 Z0.6 H15 M8
G00 Z0.2
G98 G85 X0.8295 Y-0.875 Z-0.77 R-0.065 F5.
X7.1705
G80
G53 Z0 M09
G53 Y00
M30
%

wellman91 · Feb 3, 2020

g-coder05 said:
Aside from too much wasted code it looks ok. Are you sure your tool lengths are set right?

Yes. I have measured many times and sanity checked with a ruler. Cause to me it appears to be tool offset (or something with the G gode adjusting my offset) but I know I have remeasured it many times. in the pic it is not straight on, it appears to be just shy of 7.5" when looking straight on.

BTW I use a 1-2-3 block to measure the spindle to vise(touch off). zero Z relative, insert tool manually, re touch off. z measurement goes in the tool Height offset.

Nerdlinger · Feb 3, 2020

Are you sure the Z value for your work shift is proper? Are you using G54 for the other ops, too?

wellman91 · Feb 3, 2020

Nerdlinger said:
Are you sure the Z value for your work shift is proper? Are you using G54 for the other ops, too?

yes every op is G54. its hard to see it but on a CAM preview program it shows the boring op in the correct depth. Im assuming I need to start checking parameters

13engines · Feb 3, 2020

Just for fun I'm going off topic. Like gcoder, I can't stand the crap that cam posts put out. Other then the excess trash, I also see no problem in the code.

Let's shorten that up a little more. This assumes the machine's tool change macro is worth a shit. Meaning it handles any and all preliminaries,

There are two machine movements that this shortened code will do less then written. (Eliminated useless Z0.6 TO Z0.2 moves.) Identical machining results. No loss of single block control over machine movements. And no coolant flying around while still up at the tool change position.

%
O1002 (INTEGRAL LINK)

(T15 D=1.1875 CR=0. - Z MIN=-0.77 - BORING BAR)

T15 M06 (BORING BAR)
G17G20G40G49G54G80G90

G00 X0.8295 Y-0.875
G43 Z0.2 H15 S1000 M03
M8
G98 G85 Z-0.77 R-0.065 F5.
X7.1705
G80
M09
G53Z0
G53Y0 (If safe Y0 could join Z0 in previous line)
M30
%

Cole2534 · Feb 3, 2020

wellman91 said:
Yes. I have measured many times and sanity checked with a ruler. Cause to me it appears to be tool offset (or something with the G gode adjusting my offset) but I know I have remeasured it many times. in the pic it is not straight on, it appears to be just shy of 7.5" when looking straight on. View attachment 277552 View attachment 277553

BTW I use a 1-2-3 block to measure the spindle to vise(touch off). zero Z relative, insert tool manually, re touch off. z measurement goes in the tool Height offset.

Hey! A compressor guy.

wellman91 · Feb 3, 2020

I’ll try that shortened code. I have backed up parameters that I’m going to load tomorrow, I will back up my current parameters so I can compare them. I will clear all offsets, re touch off all tools, and try to run the program again. Thanks to everyone for the help I will be posting updates, this is too weird to not follow up on.

guest · Feb 3, 2020

wellman91 said:
...BTW I use a 1-2-3 block to measure the spindle to vise(touch off). zero Z relative, insert tool manually, re touch off. z measurement goes in the tool Height offset.

It sounds to me like you're using the 2" side of the 123 block, and not accounting for it when you set your G54 Z position.

wellman91 · Feb 3, 2020

guest said:
It sounds to me like you're using the 2" side of the 123 block, and not accounting for it when you set your G54 Z position.

I use a Haimer 3D sensor for my work offsets. Maybe I have flipped the 1-2-3 block when setting tool offsets though?

wellman91 · Feb 4, 2020

guest said:
It sounds to me like you're using the 2" side of the 123 block, and not accounting for it when you set your G54 Z position.

Update: Everything is figured out. Totally user error, but it would have taken me longer to figure out with our your help, so thank you. So the 2 operations that had issues were the only tools that were measured correctly. Prior to this I had touched off all of my tools including my Haimer at once. I must have accidentally flipped the 1-2-3 block after touching off the spindle. so every operation that had tools set at that time would work as it should seeing there offsets are all equally wrong. WOW I can't believe I made such a simple basic mistake and it took this much for me to figure it out. anyways Im glad there wasn't a crash. Thanks again for everyone's help.

litlerob1 · Feb 4, 2020

Good job dude.

When this kind of shit happens to me. I stop what I'm doing, and use MDI to command Tools to places. Including Z location. Being independent of the running program, it tells me if my coordinate is set right, and if TLO is set right.

R

wellman91 · Feb 4, 2020

litlerob1 said:
Good job dude.

When this kind of shit happens to me. I stop what I'm doing, and use MDI to command Tools to places. Including Z location. Being independent of the running program, it tells me if my coordinate is set right, and if TLO is set right.

R

Yeah definitely will change how I go about solving issues like this. I was too focused on the tools that appeared to have issues seeing I had run good parts with the other tools. Lessons learned for sure.

Search

Largest Manufacturing Technology Community on the Web

Search

Could use some Help. Programming (I think)

wellman91

Plastic

g-coder05

Titanium

wellman91

Plastic

Nerdlinger

Stainless

wellman91

Plastic

13engines

Stainless

Cole2534

Diamond

wellman91

Plastic

guest

Guest

wellman91

Plastic

wellman91

Plastic

litlerob1

Diamond

wellman91

Plastic

Similar threads