4 axis confusion!

[Bill H]

I'm working on my first project with a rotary table and am way confused.  Can someone have a look at the attached files and tell me what I'm doing wrong?  The idea here is that the formed tube fits on a mandrel that's mounted to the rotary table.  The tool's Z-axis intersects with the part's X-axis (and the rotary table's axis).  As the rotary turns, the part moves along the X-axis to cut the 'scallop' feature at the end of the tube.  I have several problems: 1) Look closely at the toolpath and you'll see that it doesn't make a full 360-degree rotation around the part.  Why?  2) The first part I cut was terribly faceted.  What settings should be changed to control this?  3) Note in the G-code that the initial position of the toolpath is at approximately 180 degrees.  How can I get this position to be 0 degrees?  4) Where are those crazy feed rates in the G-code coming from?

4 AXIS CYLINDER.mcam

4 AXIS CYLINDER.NC

[mkd]

you running this on a Haas where the machine is locking/unlocking on every move, per machine parameters?

try putting an unlock code in?

[nickbe10]

19 minutes ago, Bill H said:

As the rotary turns, the part moves along the X-axis

I assume you mean the tool moves along the X- axis?

Anyway, try Arc filter/Tolerance tab.

Check the Line/Arc filtering settings box. Select all the planes you want to create arcs in and set the Cut tolerance to 0.0035 (Line arc tolerance will go to 0.00065). This should help with the faceting.

I always use derived geometry for my programs so I am not sure why selecting the solid edge doesn't complete the circle, but if you enable the Lead in / Lead out  it sorts this out, and you can add overlap (top r/h corner).

You might find it easier to adjust your start point if you use derived geometry chain as when I try and adjust the start point on your solid edge geometry it doesn't allow a start point adjustment. This can also be controlled in axis sub using the wrap / unwrap functionality.

Also you are on Bottom/Bottom and I think axis sub will normally see this as A180 as there is no defined A0 plane, I bet if you set it up Top/Top (you would probably have to rotate your part to get the correct orientation) you would start on A0.

The feed rate looks like degrees/min. You can change this output  in the post and CD.

[mkd]

the code is going from nearly a-180. to nearly a+180.. seems right to me.

[mkd]

47 minutes ago, Bill H said:

3) Note in the G-code that the initial position of the toolpath is at approximately 180 degrees.  How can I get this position to be 0 degrees? 

your toolpath running in plane bottom/bottom.

you might try playing around with your plane til it starts A0.

hint: top/front or top/back or top/top

try top/top and mess with your chain startpoint, to tweak A0. startpoint

[Bill H]

mkd:  Thanks for your replies!  Yes, I'm running this on a Haas mill with a Haas rotary.

nickbe10: Thank you!  I'm not sure what you mean by 'derived geometry'. Please explain.

[mkd]

If you create an edge curve on the part and use that for your contour, you might find it easier to adjust the start point.

 solids selection has gotten better recently, but wire frame is the tried and true method.

M10/M11  to lock unlock, IIRC. HAAS' apply the lock automatically,  so that's probably most of the faceting you're seeing

[jlw™]

I added lead in/out and overlap to fix your path but the start angle we can't change.

Added a path using curves and axis sub.

Added a path using curve 5ax.

4 AXIS CYLINDER.mcam

[jlw™]

It's probable starting on 180 because you're on Bot/Bot/Bot.

[JParis]

16 hours ago, Bill H said:

1) Look closely at the toolpath and you'll see that it doesn't make a full 360-degree rotation around the part.  Why? 

2) The first part I cut was terribly faceted.  What settings should be changed to control this? 

3) Note in the G-code that the initial position of the toolpath is at approximately 180 degrees.  How can I get this position to be 0 degrees? 

4) Where are those crazy feed rates in the G-code coming from?

1) Toolpath choice, also note, you had your unroll tolerace set to .001  I have been over this with CNC previously, really should never need to be less than the default .01"

2) There could be a couple of reasons, as noted, if the rotary is locking/unlocking try adding an unlock command at the start of the path....using the solid edge it looks like you essentially got a path on a spline and then to add the feedrate likely casued some issue as well.  Compunding the issue

3) Bottom/Bottom/Bottom as has been mentioned, try using Top/Top/Top  also, general rule of thumb, do not use bottom and back planes for positioning on a VMC rotary, create new planes by rotating and existing plane.

4) Your feed settings in your control def.....you'll have degree/per minute/Inverse and linear feed options..you will have to set this for what your machine wants, that could take some trail and error to figure out...

As far as toolpath, this is a good option for a rolldie path, especially if you do not have multi-axis ability, your file was 2017, I don't have it installed, so this is in 2018

 

old-bear_4 AXIS CYLINDER.mcam

 

N100 G20
N110 G94 G1 G17 G40 G49 G80 G90 F45.
N120 T1 M6
N130 G187 P3 E.001
N140 G94 G1 G90 G54 X-2.0025 Y0. A0. S5500 M3 F45.
N150 G43 H1 Z.935
N160 X-1.9025
N170 X-1.9007 A5.319 F2000.
N180 X-1.8968 A10.634
N190 X-1.8906 A15.943
N200 X-1.8824 A21.242
N210 X-1.8725 A26.536
N220 X-1.8612 A31.823
N230 X-1.8489 A37.097
N240 X-1.836 A42.363
N250 X-1.823 A47.628
N260 X-1.8102 A52.895
N270 X-1.7981 A58.171
N280 X-1.7871 A63.459
N290 X-1.7774 A68.755
N300 X-1.7695 A74.056
N310 X-1.7636 A79.366
N320 X-1.7598 A84.681
N330 X-1.758 A90.
N340 X-1.7611 A95.317
N350 X-1.7663 A100.629
N360 X-1.7732 A105.934
N370 X-1.7813 A111.232
N380 X-1.7906 A116.524
N390 X-1.8008 A121.81
N400 X-1.8118 A127.09
N410 X-1.8236 A132.365
N420 X-1.8358 A137.637
N430 X-1.8476 A142.912
N440 X-1.8587 A148.192
N450 X-1.869 A153.478
N460 X-1.8785 A158.769
N470 X-1.8869 A164.067
N480 X-1.8939 A169.371
N490 X-1.8993 A174.683
N500 X-1.9025 A180.
N510 X-1.8996 Z.9371 A185.443
N520 X-1.8948 Z.9389 A190.815
N530 X-1.8881 Z.9406 A196.161
N540 X-1.8798 Z.9421 A201.48
N550 X-1.8702 Z.9434 A206.73
N560 X-1.8594 Z.9443 A211.955
N570 X-1.8478 Z.9449 A217.193
N580 X-1.8357 Z.9453 A222.416
N590 X-1.8236 Z.9454 A227.609
N600 X-1.8116 Z.945 A232.812
N610 X-1.8001 Z.9443 A238.06
N620 X-1.7895 Z.9433 A243.311
N630 X-1.7801 Z.942 A248.58
N640 X-1.772 Z.9405 A253.907
N650 X-1.7655 Z.9388 A259.266
N660 X-1.7608 Z.937 A264.617
N670 X-1.758 Z.935 A270.
N680 X-1.7611 A275.317
N690 X-1.7663 A280.629
N700 X-1.7732 A285.934
N710 X-1.7813 A291.232
N720 X-1.7906 A296.524
N730 X-1.8008 A301.81
N740 X-1.8119 A307.09
N750 X-1.8236 A312.365
N760 X-1.8358 A317.637
N770 X-1.8476 A322.912
N780 X-1.8587 A328.192
N790 X-1.869 A333.478
N800 X-1.8785 A338.769
N810 X-1.8869 A344.067
N820 X-1.8939 A349.372
N830 X-1.8993 A354.683
N840 X-1.9025 A360.
N850 X-2.0025 F45.
N860 M5
N870 G91 G0 G28 Z0.
N880 G28 X0. Y0. A0.
N890 M30
%

[nickbe10]

On ‎12‎/‎28‎/‎2018 at 3:23 PM, Bill H said:

I'm not sure what you mean by 'derived geometry'. Please explain.

Derived geometry is geometry which has been generated using the solid model.

Create curve on one edge would give me a wireframe representation of the solid edge (you used the solid edge for your selection) which I can then chain as a separate entity. It has been derived from the solid.

[nperry]

On 12/29/2018 at 8:37 AM, Old_Bear said:

3) Bottom/Bottom/Bottom as has been mentioned, try using Top/Top/Top  also, general rule of thumb, do not use bottom and back planes for positioning on a VMC rotary, create new planes by rotating and existing plane.

I'm just curious why this is rule of thumb?

Thanks.

[JParis]

3 minutes ago, nperry said:

I'm just curious why this is rule of thumb?

Thanks.

You A rotation outputs will be backwards....

If you look at Top & Front the X axis runs to the right...if you look at Back and Bottom the X axis runs to the left

[crazy^millman]

Is the 4th Axis on the Right or Left side of your machine? If the 4th Axis is on the Right side of the machine then Bottom/Bottom/Bottom is correct. If the 4th Axis is on the Left side then you will want Top/Top/Top like being suggested. I think what you have should run just need to make some small changes that others mentioned and then make a good part. To get more code you will need to switch to a  5 Axis toolpath done in a 4 Axis output.

Yes the tool cuts the shape you have defined the way you have it defined and that would have cut the 360 shape. Need to look at the contact point of the tool in relationship to the surface it is machining. Change the backplot setting from endpoints to Interpolate with a .005 step increment and then you will see the exact start and stop of tool in relationship to the part. Go by what is real and not what you imagine it should be.

[So not a Guru]

On 12/29/2018 at 8:37 AM, Old_Bear said:

As far as toolpath, this is a good option for a rolldie path

Old_Bear, how do you enable the "Rolldie" toolpath?

[JParis]

It's a c-hook