Milling on a 4th axis rotary - tombstone

[hans.ivar.larsen]

Hei.

I would like to know if there's a way to enter into the cam setup a Delta x - delta y- -delta z offset from the rotary senter of the a-axsis to the measured setup point in the machine. Im used to that from Bobcad. It give you the possibility to do indexing with only one setup and you dont need to draw the hole machine setup in the cam program with the setup on in the center of rotation.

Any tips with 4-axsisn tombstone milling will be higly helpfull - links, videos and so on.

Thanks in advance

[jeff.walters]

If I'm understanding what you’re asking correctly. All you have to do is set your WCS at that point. You can do it a few ways but I prefer to put a sketch of a rectangle with one of the corners where I want the zero to be. That way I can select the XY or XZ depending on the plane it’s on.

[hans.ivar.larsen]

not sure if i got you:

Do you mean i ahve to set the WCS - setup at the center line of rotation of the 4th axsis and move the milling part Delta Y delta Z from that before i start programming?

Or could I set the WCS at the measured point at the part and move it Delta Y delta Z with the equal setoff distance measured ni the setup in the mill?

[jeff.walters]

Maybe this screen shot will help.  I created a plane 1 inch off the bottom of the model (where it would sit relative to the rotary axis). I then created an axis to represent the rotary axis. Since I wanted my X zero on the right end of the part I created a sketch on the part end. Sketched a rectangle with the top left corner (in this case) intersecting the axis. I set my orientation to be ZY, picked the vertical edge for my Z, and a horizontal edge for my Y. For the origin I changes it to Selected point and selected the top left corner of the rectangle.

The concept in our system is you don’t move the model you move the WCS. Obviously that might change if you’re working the part in an assembly of your fixtures. But then you’re not moving the model in its original file that way either.

[hans.ivar.larsen]

Dear Jeff.

I picture tells more than 1000 words. I got it - thanks. 

So I will create the setup in the machine - measure the distance from the part to be milled to the center of rotation of the 4th axsis and then move the WCS in the cam module according to the measured delta Z-Y distance.

Thanks for excelent service and assistance. Until now I admire your software!

[hans.ivar.larsen]

Dear jeff.

getting back to you with this 4Th axsis issue:

I programmed the part after your prinsipp - not a prob.

But when looking into the G-code posted I see a challange with the way its posting the angel changes.

All the indexing angels are posted positve - meaning that the rotary will turn i positive direction - make a hole turn around before it come to the correct angel. With a high fixture like I have to use - it will lead to collission and also it takes additional milling time to maek the extra moes around A.

I guess there must be away to set a kind of machine configuration in the SW - telling what way the rotary rotates when turning in positive/negative direction, and to make the rotary rotate the shortest way from the setup/start indexing angel.

Attached the G-code with notes and the fusion file

G-codes:

%

O01001 (Exctracpr-right)

(T16 D=34.7 CR=0.2 - slot mill)

(T22 D=6. CR=0. - flat end mill)

N10 G90 G94 G17

N15 G21

N20 G28 G91 Z0.

N25 G90

(Face2)

N30 T22 M6

N35 S6500 M3

N40 G54

N45 M11

N50 M13

N55 G0 A0.- This is correct

N60 M10

N65 M12

N70 M8

(2D Contour2)

N12865 M11

N12870 M13

N12875 G0 A315. - This better be A-45.

N12880 M10

N12885 M12

N12890 M9

N12895 M88

(2D Contour4)

N13150 M89

N13155 M1

N13160 T16 M6

N13165 S2900 M3

N13170 G54

N13175 M11

N13180 M13

N13185 G0 A0.

N13190 M10

N13195 M12

N13200 M88

(2D Contour3 2)

N13360 M11

N13365 M13

N13370 G0 A325.936 – This better be A-34,064

N13375 M10

N13380 M12

N13390 G17

(2D Contour3)

N13475 M11

N13480 M13

N13485 G0 A354.-This better be A-6.

N13490 M10

N13495 M12

N13505 G17

N13585 M5

N13590 M89

N13595 G28 G91 Z0.

N13600 M11

N13605 M13

N13610 G0 A0.

N13615 M10

N13620 M12

N13625 G90 G53 X0. Y0. - How to change this possition in the post prosessor? Use hompositionCenter?

N13630 M30

%

[jeff.walters]

Your best bet for post help is to go to the Autodesk CAM forum and ask the question in the Post Processors area. That way our post team will see it and be glad to help.

https://camforum.autodesk.com/index.php?board=3.0

[hans.ivar.larsen]

Hello again.

Om trying to to sign in/register at the CAM forum.

But the system are loced/blocked - disabled for register. It has been this status for a long period.

Do i do something wrong or am I at the worng site.

https://camforum.autodesk.com/index.php?action=register

[jeff.walters]

I have asked our Post team to reply to this form insted. 

[AchimN]

Look for this code into your post:

  if (true) {
    var aAxis = createAxis({coordinate:0, table:true, axis:[-1, 0, 0], cyclic:true, preference:1});
    machineConfiguration = new MachineConfiguration(aAxis);

    setMachineConfiguration(machineConfiguration);
    optimizeMachineAngles2(1); // map tip mode
  }

By changing -1 to 1 you are changing the direction of your a-axis which should fix your problem.