Help with program

sidetrack50 · Nov 5, 2018

Well I guess my machine works ok but I definitely need help programming. Can you guys look this over and see where I'm going wrong. The program works up to block 10 where it mills straight to Y 4.8125 after milling the circle but when it goes to X 5.375 it goes rogue and mills straight while making a small curve at the end, ends up at X 5.660, tried changing things but it doesn't help.

VTM · Nov 5, 2018

Can you post a shot of the actual program on the machine screen. And whats in D8? Most people probably wouldn't call g41 D8 at the first position call, but I'm not sure that's your problem.

sidetrack50 · Nov 5, 2018

VTM said:
Can you post a shot of the actual program on the machine screen. And whats in D8? Most people probably wouldn't call g41 D8 at the first position call, but I'm not sure that's your problem.

D8 is the cutter comp for tool 8 which is dia .570, here's the program on the machine.

VTM · Nov 5, 2018

Its N10 you've called D8 Twice without canceling it the first time for one. Remove E1, D8,G41,G90 from your N10 line and you should be good. You should have a safety line at the beginning of each tool IMHO That .contains G80 G90 G40 at least

sidetrack50 · Nov 5, 2018

I added more info on line N10 but it didn't help, before it was just Y 4.8125 and N11 was X 5.375

VTM · Nov 5, 2018

Hers a sample Fadal program for you. Maybe you can get some pointers from it.

guest · Nov 5, 2018

I don't see the G1 in N7 or the G2 in N9...

The X5.66 endpoint is correct- G41 is still active and the next move in N12 is the Y move to 3.1875. The endpoint of X5.375 has 1/2 of .570 added to it, which puts the center of the spindle at X5.66. The little arc at the end of N11 is just the control swinging a .285" radius around the corner.

VTM · Nov 5, 2018

You don't need to add more info. get rid of the E1, D8, G41 and G90 at line N10.

VTM · Nov 5, 2018

guest said:
I don't see the G1 in N7 or the G2 in N9...

The X5.66 endpoint is correct- G41 is still active and the next move in N12 is the Y move to 3.1875. The endpoint of X5.375 has 1/2 of .570 added to it, which puts the center of the spindle at X5.66. The little arc is just the control swinging a .285" radius around the tool radius.

He has G2 at N9, But your right he does need a G1 at N7

guest · Nov 5, 2018

VTM said:
He has G2 at N9, But your right he does need a G1 at N7

Oh, you're right- it's at the end,lol.

Not the way I write my progs, but it's not a rogue machine- the moves are correct for a value of .570 in the D8 register. If the OP single blocked through, he would see the same shifts on the other end points.

sidetrack50 · Nov 5, 2018

VTM said:
He has G2 at N9, But your right he does need a G1 at N7

Ok, this works perfectly up to line 11, it mills the circle then moves to Y4.8125 then moves to X 5.375 but has the curve at the end, it should stop at the X position then go straight to Y 3.1875

guest · Nov 5, 2018

sidetrack50 said:
Ok, this works perfectly up to line 11, it mills the circle then moves to Y4.8125 then moves to X 5.375 but has the curve at the end, it should stop at the X position then go straight to Y 3.1875

Um, no. It will feed a line to X5.375, then swing a .285" radius around that point (X5.375 Y4.8125). Then it will feed straight down to Y3.1875 with the center of the spindle at X5.66. This puts the edge of the tool at X5.375, which is what you are asking it to do.

VTM · Nov 5, 2018

Are you actually cutting a part? Or your just seeing the arc by watching the control?

N11 is just the control swinging a .285" radius around the corner.

sidetrack50 · Nov 5, 2018

guest said:
Oh, you're right- it's at the end,lol.

Not the way I write my progs, but it's not a rogue machine- the moves are correct for a value of .570 in the D8 register. If the OP single blocked through, he would see the same shifts on the other end points.

HaHa....not a rogue machine just that last move at N11, it should be millng straight lines until the next part where it goes into another circle.I have 6 straight moves after the first circle.

sidetrack50 · Nov 5, 2018

guest said:
Um, no. It will feed a line to X5.375, then swing a .285" radius around that point (X5.375 Y4.8125). Then it will feed straight down to Y3.1875 with the center of the spindle at X5.66. This puts the edge of the tool at X5.375, which is what you are asking it to do.

Doesn't G1 cancel the G2, I'm .100 above the part checking its path before I cut

VTM · Nov 5, 2018

Yes but your in G41 with a comp number entered. So the machine is comping like it should. Drop your tool down and skate .005 off that part and see what you get.

sidetrack50 · Nov 5, 2018

VTM said:
Hers a sample Fadal program for you. Maybe you can get some pointers from it.

VTM....That program is what I'm trying to do go from G2 to G1 but I get that radius move on line 11 when it's in G1 mode, am I missing something?

VTM · Nov 5, 2018

The program looks good to me at this point. I'm not there so I can't see what your seeing. Is it swinging a BIG radius? Best thing to do is to drop the cutter down and just kiss the top of the part. See what the cut pattern looks like.

sidetrack50 · Nov 5, 2018

VTM said:
Yes but your in G41 with a comp number entered. So the machine is comping like it should. Drop your tool down and skate .005 off that part and see what you get.

It still does the same and if I go to line 12 it makes a small half circle

sidetrack50 · Nov 5, 2018

VTM said:
The program looks good to me at this point. I'm not there so I can't see what your seeing. Is it swinging a BIG radius? Best thing to do is to drop the cutter down and just kiss the top of the part. See what the cut pattern looks like.

It makes about a .5 radius, is there something I should use to stop the g2 code cause its making radius's.

Help with program

Aluminum

Hot Rolled

Aluminum

Hot Rolled

Aluminum

Hot Rolled

Attachments

guest

Guest

Hot Rolled

Hot Rolled

guest

Guest

Aluminum

guest

Guest

Hot Rolled

Aluminum

Aluminum

Hot Rolled

Aluminum

Hot Rolled

Aluminum

Aluminum

Similar threads