SP1 Helix Bore

[?Mark]

It's posting with a bunch of linear moves (on the same z) at the beginning and end of this toolpath.

 

Before (V9 and before sp1) I had a clean move from a center to the wall, then circular full arcs to the bottom, linear move to the center and retract

I just can't to get it to work like that anymore

Any help appreciated

 

Mark

[?Mark]

Those linear moves are forming full circle (half the programed dia) going clockwise at z.0 and then it does helical downward (as it is supposed to) and again linear exactly like on the top of helix...

 

Mark

[DavidB]

Filter is on?

[?Mark]

Output arcs is checked.

The main toolpath looks good, but the beginning and end

Even backplot doesn't show those linear moves

 

here is a sample of code:

 

G54G0G90X0.Y0.

G43H3Z2.

M8

Z.1

G1Z0.F25.

G41D3Y.0705

Y.141

 

and a bull$#@t starts

 

X.0163Y.1391

X.0316Y.1335

X.0453Y.1245

X.0565Y.1126

X.0647Y.0984

X.0694Y.0827

X.0704Y.0664

X.0675Y.0503

X.0611Y.0352

X.0513Y.0221

X.0387Y.0116

X.0241Y.0043

X.0082Y.0005

X-.0082

X-.0241Y.0043

X-.0387Y.0116

X-.0513Y.0221

X-.0611Y.0353

X-.0675Y.0503

X-.0704Y.0664

X-.0694Y.0827

X-.0647Y.0984

X-.0565Y.1126

X-.0453Y.1245

X-.0316Y.1335

X-.0163Y.1391

X0.Y.141

 

good part

 

G3J-.141Z-.1

J-.141Z-.2

J-.141Z-.3

J-.141Z-.4

J-.141Z-.5

J-.141

 

and a bull$#@t starts

 

 

G1X.0163Y.1391

X.0316Y.1335

X.0453Y.1245

X.0565Y.1126

X.0647Y.0984

X.0694Y.0827

X.0704Y.0664

X.0675Y.0503

X.0611Y.0352

X.0513Y.0221

X.0387Y.0116

X.0241Y.0043

X.0082Y.0005

X-.0082

X-.0241Y.0043

X-.0387Y.0116

X-.0513Y.0221

X-.0611Y.0353

X-.0675Y.0503

X-.0704Y.0664

X-.0694Y.0827

X-.0647Y.0984

X-.0565Y.1126

X-.0453Y.1245

X-.0316Y.1335

X-.0163Y.1391

 

good part

 

X0.Y.141

G40Y0.

G0Z.1

M9

 

Can someone give it a shot and create simple helix toolpath to see what's happening?

 

Thanks

 

Mark

[DavidB]

This does not answer your question but can you use contour ramp toolpath instead? I use this toolpath to do all my circular interpolation toopathing of round holes.

 

Maybe check control settings under Arcs/Support arcs in XZ plane is it ticked?

[?Mark]

David,

I use this toolpath too and it works great, but if I have points ready I should be able to create helix bore with it.

For contour ramp I need to create additional geo (circle).

I know, not a big deal, but why create something you don't need...

 

Mark

[DavidB]

Maybe check control settings under Arcs/Support arcs in XZ plane is it ticked?

[jeff]

Works fine here.

Have you tried a different post configuration?

[?Mark]

You guys running sp1?

All was good here before sp1...

 

Mark

[DavidB]

Works here too... SP1

 

G00 G17 G21 G94 G90

G40 G49 G80

T219 M06 ( 10. FLAT ENDMILL)

M97

M56 H1 D2

G54

G00 G90 X10. Y0. S4000 M05

G43 H1 Z10.

G01 Z0. F3.6

X19.998 Y-.175

G03 X20. Y0. I-9.998 J.175

X-20. Z-2.5 I-20. J0.

X20. Z-5. I20. J0.

X-20. Z-7.5 I-20. J0.

X20. Z-10. I20. J0.

X-20. I-20. J0.

X20. I20. J0.

X19.998 Y.175 I-10. J0.

G01 X0. Y0.

Z10.

M05

G91 G00 G28 Z0.

G91 G28 X0. Y0.

M11

G91 G28 B0.

M82

M99

%

 

A guees something is up with your control def.

 

Email your file to me I'll post it here if u like?

Use the zip2go utility under help

[?Mark]

Should be inbox just about now.

Thanks

Mark

[DavidB]

Mark,

Did you tick Toolpath files,Post processors when you zipped the file?

Theres nothing with your file not even Geom.

[?Mark]

Everything should be there.

 

Mark

[DavidB]

Ok whats the best way to open the .Z2G file?

[?Mark]

Look here link

 

This .Z2G is a .ZIP format file that you can open and manipulate with WinZip.

 

David, I'll be going home soon.

Maybe tomorrow will end my brain fart

Mark

[DavidB]

Marc ,check email...

This is what i got using your post,machine and control def...

%

O1300

N100 G0 G17 G40 G49 G80 G90

M6

S1426 M3

N110 G54 G0 G90 X-.5 Y.0705

N120 G43 H3 Z1.5

N130 Z1.4

N140 G1 Z1.3 F6.33

N150 X-.4295

N160 G3 X-.5 Y.141 R.0705

N170 J-.141 Z1.22

N180 J-.141 Z1.14

N190 J-.141 Z1.06

N200 J-.141 Z.98

N210 J-.141 Z.9

N220 J-.141 Z.82

N230 J-.141 Z.74

N240 J-.141 Z.66

N250 J-.141 Z.58

N260 J-.141 Z.5

N270 J-.141 Z.42

N280 J-.141 Z.34

N290 J-.141 Z.26

N300 X-.359 Y0. J-.141 Z.2

N310 I-.141 F1.9

N320 X-.4295 Y.0705 R.0705

N330 G1 X-.5 Y0.

N340 Z1.4 F6.33

N350 G0 Z1.5

N360 G91 G28 Z0 M19

G28Y0

G53G90X-16.0

G90

N370 M30

%

 

Look at the last toolpath I added a helix bore toolpath.

Above is the posted code

[?Mark]

Thanks David.

So in other words, the same toolpath with the same post, control/machine definitions gives us different code

I'm running level 2 with solids here.

Somebody willing to chip in as to what I'm doing wrong here?

 

Thanks

Regards, Mark

[DavidB]

In the file you sent me you did not have a helix bore toolpath.I sent the file back to you with a helix bore toolbar in it.Take a look at it and see if its different to what you where doing.Post it at your end and see what you get.

HTH

[?Mark]

quote:

---

In the file you sent me you did not have a helix bore toolpath.

---

I deleted them and used contour ramp, because helix bore gave strange code.

quote:

---

I sent the file back to you with a helix bore

---

David, I didn't get anything

 

Mark

[Jon Griffin CNC Software]

A situation like this has come up before, and we tracked down an incorrect setting. Please check the following:

 

they determined that MachineTypeControlDefinitionArcArcErrorChecksParallel axis motion on quadrant checkbox had been checked in the submitter's control definition. This caused the arcs to be linearized when written to the nc file.

 

 

If it is checked, uncheck it, and try posting again.

 

Jon Griffin

Software Engineer

CNC Software

[?Mark]

Thanks Jon, but it's unchecked here

?

 

Mark

[MLewis]

I'm working on the same problem. I have 4 locations in the operation, the first two have linear moves (a pt2pt circle) before the helical code, the last two locations have correct ouput?

 

I'm not getting any linear moves at the end of the operation.

 

The post is going into plin$ instead of pcir$ for some reason?

[kccadcam]

Try changing: General Math function tolerance from

.0001 to .00005 in control def.

[DavidB]

Resent email

I used your control def,machine def and post, and I got arc moves. So I think it might be something in your toolpath parameters.Have a look at the Helix toolpath I did and post it at your end ????

[?Mark]

David, got your email and figured what's up here.

Here is what I get:

G0X0.Y0.

Z.1

G1Z0.

G41D1X.125

Y-.125

G3X.25Y0.R.125

I-.25Z-.1

 

Works fine with your setting:start angle 0, entry/exit arc sweep 90.

 

just don't understand why I can't get it to post as before (V9):

Here is a code I can't get to post:

 

G0X0.Y0.

Z.1

G1Z0.

G41D1X.125

X.25

G3I-.25Z-.1

 

Not sure why that is

 

Thanks, Mark

 

BTW changing General Math function tolerance from

.0001 to .00005 in control def. didn't make a difference.