Helical toolpath

[SBA]

I have done this before but seems like it wont work now? If I create a helix in the top plane going down in Z. I then use this as the toolpath and apply a filter to create arcs in XZ and YZ planes. Should this not then create a helical toolpath. Example G17 G3 XYZ. With or without the filter it is creating XYZ moves over the toolpath.

In V9.1 Mill

[connormac]

Don't you almost have to have an XYZ move in a helical path. I might be wrong(big shock) I have only used it 1 time.

[Hardmill]

quote:

---

and apply a filter to create arcs in XZ and YZ planes.

---

These planes have nothing to do with a helical toolpath

in the XY plane (G17). Create arcs in X-Y

 

 

PEACE

[BernieT]

You can get a helical toolpath by using Pocket, helix entry, 'follow boundry'. Set a BIG stepover and you will get only the helix. Be sure the post processor is set to 'Output helix' in the debugging and switches section. You will get G2 XYZ IJ output in the NC file.

 

Don't know why the 3D contour toolpath won't give G0 XYZ IJ NC code......

[Kelly Burns]

Why cant you just chain your geometry and use the ramp down feature? Isnt this the same as creating a helix. We use it all the time for ripping out and finishing ops on pockets.

[Müřlıń®]

quote:

---

Why cant you just chain your geometry and use the ramp down feature? Isnt this the same as creating a helix.

---

+1... that is why there was no more reason for thelix.dll.

 

 

So now all you have to do is draw a 2-d circle and use the ramp to set your helix. lots easier now

[SBA]

I think there may be some confussion on my question. The code output is actually doing the same thing just is alot more code than needed. I was thinking in the past that the filter converted all the small moves to a single helical move line. I want a helical move around a inside diameter but not full circle such as thread milling.

 

Example:

 

N10M98 P9810

N20T99

N30T10

N40

(TC T10; CALLUPT10END PROGRM)

N50

N60M6

N70G0G20G17G40G49G80G90G54

N80M3S1069T10

N90G0X-.1377Y1.6472

N100G43H10Z.25

N110M8

N120Z.1

N130G1Z-.05F6.42

N140X-.1584Y2.1468

N150X-.0249Y2.1523Z-.0523

N160X.0348Y2.1522Z-.0534

N170X.1622Y2.1464Z-.0558

N180X.2223Y2.141Z-.0569

N190X.3488Y2.124Z-.0593

N200X.408Y2.1135Z-.0604

N210X.5326Y2.0856Z-.0627

N220X.5907Y2.0699Z-.0639

N230X.7123Y2.0312Z-.0662

N240X.7688Y2.0105Z-.0673

N250X.8866Y1.9614Z-.0697

N260X.9411Y1.9358Z-.0708

N270X1.0542Y1.8766Z-.0732

N280X1.1062Y1.8464Z-.0743

N290X1.2138Y1.7776Z-.0766

N300X1.263Y1.743Z-.0777

N310X1.3641Y1.6651Z-.0801

N320X1.4101Y1.6263Z-.0812

N330X1.504Y1.5398Z-.0836

etc.

 

As apposed to this

 

G17 G2 X-2.0281 Y-1.288 I.1687 J-2.3966 Z-.216

 

The top code is what I am getting the bottom is what I was looking for. Both will work. Thanks all for replies.

[Thad]

Is "linearize arc moves" checked?

 

Thad

[SBA]

Thad

Not that I can find anywhere in the operation.

[Thad]

Just a guess. I'm not sure if that option is even there. I've never cut a helix. I've always use contour-ramp, as others have suggested.

 

Thad

[Craig-B]

Hey SBA,

Try checking the following settings in your post.

do_full_arc : 0 #Allow full circle output? 0=no, 1=yes

helix_arc : 2 #Support helix arc output, 0=no, 1=all planes, 2=XY plane only

arccheck : 1 #Check for small arcs, convert to linear

[Bobkat]

Another place that you might look is under the “Control Definition” that is being used by your Machine Definition.

Go to the Arc category, and over to the right side of that page there is an area for “Helix Support”. There are 3 choices.

Toggle "All Planes Supported" and see if that gets you what your after.

Good Luck

Bob

[Bobkat]

Whoooops ... wrong product ...never mind

Sorry

Bob

[SBA]

FNMI, Tried post settings does not seem to be it.

do_full_arc normally i leave set to 1 but changed to 0 no differance.

helix_arc : 2

arccheck : 1 , was 3 changed to 1 no differance.

Bobkat

I have software and code but key is in upgrade process.

I think it is because it is a parametric spline. I read a post in search that was very similar to this. Tanks all for time.

[Craig-B]

If its a parametric spline then you will not get arcs moves, you will get all XYZ moves. I think that it's because Mastercam doses not see splines as arcs. Maybe some one here on the fourm can explain it better.

[?Mark]

Modify/convert to arcs?

 

Mark

[kinglouie V]

what I want to know is where in the hell this function is getting it's ccomp command from it's driven me nuts. It is NOT looking at pcancelcc, otherwise it would output a G1 in front of G40.

The Okumas (at least these) will not pick up or dump comp. in an arc so I need it this way.

[connormac]

SBA,

When you draw your helix. It will ask you how many degrees to up date. the smaller the number the more times it will produce code. Just increse the number of degrees between update. HTH