MILL/TURN AGAIN

[DavidB]

Hi all,

 

Im not asking 4 a post.OK

 

Im trying to machine a square on the end of a turned part. LB15 Okuma Lathe Turn machine.

 

I set C/plane and T/plane to 3 (back). Countour mill toolpath a single line.

Do the same in Top,Front and Bottom and i should get a sqaure?

 

What I get in backplot is the part spinning on the c axis.

The C axis should be set to C zero,90,180,270 and the cutter move in Y axis.

What am I doing wrong?

 

Also the post MPOSP7C.PST spits out a whole lot of C axis moves.

 

Thanks for any replys

[gcode]

In the Rotary Axis box, change the Rotary Type from C to Y. I'm not familar with the post you

are using so I don't know if it supports Y axis milling or not. If it is outputing C axis moves, it probably does, but you may have to enable the Y axis.

This is a cut and paste from the newest MPLFAN post

 

# --------------------------------------------------------------------------

# Machine Specific Settings

# --------------------------------------------------------------------------

#Machine axis switches, initial

y_axis_mch : no #Machine has Y axis, 0=no, 1=yes

[Glenn Stephens. from CCCS]

Top front and bottom are not the correct planes. Use the cview c-hook and set your C axis values to get the appropriate planes. Also, in the toolpath, you need to go to rotary settings and set it to Y-axis. The post must also be set for y-axis: y_axis_mch : 1

[gcode]

Too slow Glen

 

BTW, I got CATWRITE to work by uninstalling and reinstalling it this morning. Thanks for the help!!

[DavidB]

this is what's in my post.

 

y_axis_mch : 0 #Machine has Y axis

 

should i change it to a 1???

 

thx 4 the reply's guys

[tryon]

yes, and i think you need to do this in the top tplane

[Reece L Gibson]

Sounds like you are wanting to lock the "C" axis and mill in the "Y" axis Correct?

C0 is view #3.If you set the Cplane and Tplane and the Gview to #3 and mill you contour it should post correctly(if you have the post for your machine).From here you can rotate the tool path or use your Alt and arrow keys to rotate the part towards you or away from you(around the "Z" axis),towards me is C pos on the Hicell.I use this to teach how the C axis works in MC. Every press of the arrow key rotates the "C" axis 5 degrees.When you get to where to geomerty is perp to you, mill your contour with that tplane and cplane active to the current view.

It will then output the "C" axis and mill your contour. Think as if your are the tool, and the part rotates underneath you.You can do this other ways, but if you do not get the tplane right it outputs wrong code.Be sure to have your Misc set to Y axis motion as the other members have mentioned.

Hope this helps.

 

 

Good to see you back on here Glenn

[DavidB]

I changed it to a 1 and i get this in posted nc file.

 

Ex:G94 G1 X18.101 C51.216 F700.

N118 X17.75 C52.648

N120 X17.413 C54.125

N122 X17.091 C55.647

N124 X16.783 C57.215

N126 X16.491 C58.828

N128 X16.213 C60.487

N130 X15.952 C62.191

N132 X15.707 C63.939

N134 X15.478 C65.73

N136 X15.265 C67.563

N138 X15.07 C69.436

N140 X14.892 C71.347

N142 X14.761 C72.913

N144 X14.642 C74.505

N146 M16

 

T/plane and C/plane set to #3

[DavidB]

What am i missing it should be y axis movment only at C0???

[Reece L Gibson]

On the Rotary button,check to make sure the "Y" axis is on,not the "C".In my last post I was assuming you want to use a Live X tool.

Here a same of a Hicell code:

(SURFACE ROUGH POCKET LIVE X)

N20 G30U0V0W0M45

T101000

M43

G28H0.

G50C0.

G19M44

G0G97S3000M13

C270.

G0X2.7925Y-2.0167Z-3.6249M8

G98G1X2.5925F25.

Y-1.5167F15.

Y1.5416

Z-3.2854

Y-1.5167

Z-2.9459

Y1.5416

Z-2.6064

Y-1.5167

Z-2.2669

Y1.5416

I have 4 1/8" of travel in the Y

[DavidB]

I changed all settings that u told me,what i missed was turning misc interger on.

(Y axis over centre ON OFF.)

If i set this I get what im after if I dont I get all the C axis movement.

 

This is what i get now Thank you very much

 

 

O0000 (TORQUE_TUBE_BLANK )

NAT09

( TOOL - 9 OFFSET - 9 )

( CONTOUR 3/8" TC TIN COATED END MILL )

N100 G13

N102 G0 X0. Y400. Z-250. M05

N104 M110

N106 G138

N108 T0909 SB=1900 M241 M13 M86 M8

N110 G0 X25.912 Y7.055 Z-4.523

N112 C0.

N114 X11.912

N116 G94 G1 X3.912 F700.

N118 Y1.816

N120 Y-1.943

N122 Y-7.182

N124 G0 X23.912

N126 M9

G136

N128 M12 M02

 

This program was at C/plane and T/planeset at #3

 

But im still having trouble trying to machine the other 3 faces of the square???

[DavidB]

MILLTURN

quote:

---

Sounds like you are wanting to lock the "C" axis and mill in the "Y" axis Correct?

---

Thats exactly what I want to do.

I have done face at C/Pplane and T/plane #3 (back).

If i have an ISO view and select the line that represents the top face of the square,how do i get the C axis to rotate to the T/plane and machine in the Y axis?

 

Its not a square as such the four sides are different dim from the centre line so i cant rotate the toolpath.

 

Thx

[tryon]

how about try using section chains all going the same direcrtion.

[Harryman]

David, best way I know to get the Cplane correct is to set the Cplane at each face with two right angle lines that form the correct Cplane. Select X axis first then Y. It's easiest if the lines intersect at one endpoint but not mandatory. It is a more bulletproof method than selecting named Cplanes for me.

[Harryman]

David, if you set Cplane to Top and do Cross drilling, what angle does C axis go to?

 

Sorry to post a question and then run away but it's geting late here. Clarification will help someone else help you too. G'night.

[DavidB]

The tool stay's in T/plane #3 (Back).

I was under the impresion if i selected a line that was laying in the top C/plane,the C axis would rotate 90 deg to the tool plane?

I think i need to make any new C/planes as its just a square that is perpendicullar to the y axis.

 

Cheers

[Harryman]

Ok, Try starting from Cplane Back, Click on Cplane then select rotate aboput Z axis 90 degrees and see what you get. I can't try it at home and I haven't tried this at work. Just a thought. It works well rotating the Cplane about Z when staring from Side Cplane.

 

The Tplane has to also be independently changed to match the Cplane. Just set it to the same # that appears when you save the Cplane.

[gcode]

David,

You'll need to build a toolpalne for each wall you want to cut.

I would rotate TP#3 by clicking the Tplane Icon

then Rotate. That will show you a visual of TP#3

and give you 3 different ways to rotate it.

When you get it to rotate the way you want click Save

Then go into WCS, right click in the chart and click Save currrent Tplane. It will take a little trial and error.

Once you get this job right, save the Tplanes as an empty file.

The next time you need to mill 4 faces 90 degrees apart you can import them through Job Setup/Import Views. If you save them the first time, you'll never have to build them again

[DavidB]

T/plane #3 is the standed (Back View).

I dont need to create any special t/planes to machine this job.

 

The other 3 faces then would be on the standard Top,Front and Bottom T/plane and C/plane.

 

I just cant get the C axis to rotate 90 degrees when machining the top C/plane geomertry.

 

 

[lathe guy]

i think u need to use a seperate cplane/tplane for each c rotation. this should force the c rotation. when doing this make sure to check the c plane that z and y are in correct directions according how tool will be aproching part at c rotation

[Harryman]

Sorry David, my last post was BS, about rotating. It works when starting from the side Cplane and rotating about Z but I couldn't find a way to rotate Cplanes the way you need to. This is the technique that you need to use if you have a part feature on the face (side Cplane) and need to align it(in C) with the X machine axis to reach it due to machine travel limit issues.

 

EDIT: I need to experiment more with those rotation features.

 

Lathe guy is right. If you want to machine on multiple faces (various C axis positions) with X axis tool approach (tool pointing to chip pan) you need to use a different Cplane/Tplane for each face, and my personal experience is that the best way to set them is to select geometry rather than names.

[crazy^millman]

Can I ask a dumb question here does it have a transform fucntion and could you just transfrom the one operation 4 tiems around the part for each side of the square?

[DavidB]

Millman I could and edit the deepth on each face to get the dim im after.But I want to know how I can get it to work in M/C.

 

Lathe guy if i use top T/plane and c/plane mastercam backplots correctly but the tool is in the top not at the back and this doesn't put in a C axis rotation.

 

[Harryman]

quote:

---

if i use top T/plane and c/plane mastercam backplots correctly but the tool is in the top not at the back and this doesn't put in a C axis rotation.

---

Could it be a post thing?

 

For me, machining done on Top Cplane posts code positioning Caxis to 90 Degrees, as it should in my opinion.

 

Does your post output C zero degrees for work done on Back AND Top Cplane/Tplane?

[DavidB]

Ok im at work now.

Im trying to machine the top face of the square.

I set T/Plane back #3 C/plane top.

The toolpath backplots with the tool moving along the contour in x axis.It should even in backplot rotate the job 90 degree and move in the Y axis I think?

I have set the rotary button to Y.