Need Help!- C axis maching problem

[SmokinErb]

I drew my part on mastercam x. It has 8 face holes and an angular slot on one of the holes. I run the graphics and everything looks great, but when i post and put program in the machine. It drills the holes but when it cuts the slot the angular position is WAY off. G54 C = 0.000 there is a G28 H0 before both tools. I can't figure this out. could someone please give me some ideas. Also when i interpolated the holes with the same endmill that is cutting the slot, all the locations were fine, It has something to do with it being seperate tools.

[Stebedeff]

Are you a experienced mastercam C-axis user? I do a lot of C-axis myself with or without mastercam. First of all make sure your part is on the good WCS which is usely with standard lathe the Right WCS. The 3 O'clock is your C-axis zero. Maybe you know all this already. About your angular slot, i have an idea of what it looks like but a file or picture would be best. Are you using a contour toolpath for your slot? Straight line or contour? Is your cutter compensation set on control or computer? What machine control are you using? Just asking to have an idea.

[cnc-king]

g28 h0 will send the c axis home on most fanuc's control that i have worked on
h is the incremental call for the c axis.
if you are milling on the face of the part you WCS should be set to D+Z+ and your Cplane & Tplane should be Right. if you are using the caxis tool paths in master cam the software automatically sets those for you. if you are using the milling option in the lathe you have to set those your self by opening the planes window in the toolpath parameter.

[SmokinErb]

I'm still newish to mastercam. I've been sucessfull with milling on c. I am not able to show a print. So i just drew a little sketch. The slot/cut-out is 90 Deg (+/- sum) from the drilled holes. I've drawn it and programed it from the Right side view. the Graphics look perfect, It does exactly what i tell it to do. I also programed it with Interpolating the holes with the same Endmill that does the cutout, and it came out normal, but the holes where oversized and i wanted to drill them. Its Delrin .700Dia the holes are .085 +/- .001 I changed the drill cycle in the program from G54 to G56 (since G55 is my sub spindle after transfer) set the same Z and input 90. in the C and it came out close to being good. I had to leave so in the morning i will CMM it and move my G56 C offset accordingly. But I want to understand what mastercam is thinking. I have to be missing something. Maybe if I had a real working post i wouldn't have this problem, but my company will not purchase posts. Its amazing the company will but Nice Mori Seiki Machines, Mastercam, but they don't think the posts are nessasary. I wish i could make my own. Any help would be greatly appreciated.

[SmokinErb]

here is a much better sketch, can someone please help

[SmokinErb]

Here is my MCX file

[cnc-king]

your file verifies fine the cut out is in the correct orientation. what seems to be the problem?

the only problem with the way you did it is the numbers in backplot shows radial values instead of diametrical


take a look at this file i changed your top WCS to the D+Z+ wcs and the verify is the same, you probably will need to change multi pass and d.o.c etc.

[SmokinErb]

The problem is when i take a finished part out of the machine, if i put the part on the table, just the way it is drawn on the second professional sketch, the milled cut out is rotated 90Deg. Counter Clockwise than where it is sopposed to be. This causes a couple holes on the left of the part to be cut away. Its driving me nuts on why it would be like that, since the graphics in MC look great

[Superman]

You have created a program that does not require much modification.

OK, you have a relationship problem with WCS, C and T planes. It's how you are programming the part, the planes you are selecting for the milling tool are at fault ( Top and Right sides ). I think your TOP should be BACK (3 o'clock position).

Read the header section of your selected post for planes used for milling TOP and for RIGHT views

What post are you using ?
If you are not sure, paste in the top dozen lines

[Stebedeff]

I've checked your file and generated a G-code. The problem is that the G112 code is after the C92.973 ( first C-axis move ). I´am guessing you have a Fanuc. One thing you should know about C-axis using G112 is that before you use G112 you can position your C axis anywhere you want. From then it will mill your program under the G112. Even if you program your path in absolute. The path is increment from you C-axis position. Kind of difficult to explain for me. A better way to understand.....Say you have a 10 inch round disk. And you want to have squares milled every 60 degrees or whatever you wish. You program your square ( path ) in a subprogram using G112. Use G112 before all X or C axis move. Then in head program you can call up the 1 subprogram at any Degree you want.

Your problem with the part is the C92.973. From this point on it will execute the contour you want. And that's why you contour is exacly 92.973 degrees off.

You should start the G112 and your program at C0.0 Why zero? Because that's your drill path zero as well.
So best if you put in a start point ( lead in from point )at 0.0 degrees befor you go to your first contour entity. But draw a line to your path and back. Make it a closed contour.

[SmokinErb]

Stebedeff That was it, I drew that other line from C0 and away i went, Thank you EVERYONE for your help. CNCZONE is best