Trunnion Set Up

Disclaimer
Use at your own risk, these are the steps I took to set up my machine only It may not work on your machine. If you choose to follow these steps on your machine do so at your own risk. By following these steps you agree that I makingchips in no way liable for mistakes or damages caused to you or your machine.



Setting up the TR 160

1. Once you put the A,B table on the machine table with bolts (snug not tightened) indicate the very front of the platter at horizontal (platter facing the Z axis) when you touch the front of the platter zero out the indicator write down the Z number displayed on the control. (or even enter it into the G54 offset) Retract your Z to a safe distance.

Now move in Y to the back of the platter bring your indicator down and touch the platter in .0001 mode until the indicator reads zero. Take down the Z number on the control and find the difference between the two numbers. Take the new number and divide by two. The new divided number is what you will need to move the A axis to make it flat.

Once you move the A axis to that number indicate across the face to verify it is now sitting flat across the Y axis. If it is 0 across enter it into G54 for the A axis. You may have to do this step again later after you tighten down the A,B table to the machine table remember at this time it is only snug.

2. Rotate the A axis to 90 degrees vertical (platter facing you) as displayed by the G54 position not Machine position. Indicate across the face of the platter in the X axis the same way you would if you were indicating the jaws on a vise, tapping with a rubber dead blow until the indicator reads zero across the X axis. Tighten the bolts holding the A,B table.

3. Rotate the A axis back to the G54 offset zero and indicate across the platter and verify it is still 0 on the indicator across Y, if not redo step 1.

Finding the center of rotation for the Z tool height offsets.

1. Using your trusty .0001 indicator find a spot on the machine table you can get to with the Z axis ( hint I used Joe blocks) zero out the indicator once you touch the table, and take down the Z number displayed on the control. ( if you used Joe block make sure you add this to number you wrote down).

2. Bring the Z axis back to a safe distance. Tilt the A axis to the G54 90degrees. Put a 1.4995 pin into the center of the platter. Touch off the pin until your indicator reads zero. Take down the number for Z displayed on the control. Add half the diameter of the pin to that number. The difference between the first Z number taken from the table and the last Z number taken from the pin is the number you will need to set the tip of your tools too. I made a block ground to that number minus .100 bolted it to the machine table. I use that and a .100 Joe block to set my tools.

Finding the difference from the platter top to the axis of rotation (used for cam) ***Copied from the Haas manual Page 8 and 9 VF-Series Trunnion manual***


This procedure determines the distance between the plane of the B-axis platter and the A-axis centerline on
tilting rotary products. Some CAM software applications require this offset. It is not used by the Haas control.
1. Rotate the A-axis until the B-axis is vertical. Mount a dial indicator on the machine spindle (or other surface
independent of table motion) and indicate the platter face. Set the indicator to zero.
2. Set the Y-axis operator position to zero (select the position and press ORIGIN).
3. Rotate the A-axis 180°.
4. The platter face must now be indicated from the same direction as the fi rst indication. Place a 1-2-3 block
against the platter face and indicate the face of the block that rests against the platter face. Move the Y-axis to
meet the block with the indicator tip. Reset the indicator to zero.
5. Read the new Y-axis position. Divide this value by 2 to determine the B on A axis offset.

Makingchips

Click to expand...

Originally Posted by DRD
I have a vf 3, with a 5 axis trunion table. The set up is no different than your fadal, all the offsets are based off Zero. We also use mastercam x3 for programming.

I will tell you, ignore the dimension haas gives for there center line A rotation.
I chased set up problems for days, going off the Haas information, to find out my center line was .027 shorter than what haas specs in there info, in inverse time, this becomes a polar problem. I had to measure everything to find the problem.

Also you will need to change parameter 85 in the control, for 5 axis work correctly. When you get the machine set up and making parts, you might need to tweak the back lash steps in the control for A and B also, this becomes a judgment call on 5 axis machining for sure.
Good Luck.


I'm taking it that the following is what you are talking about?

"Settings
A number of settings are used to program the 4th and 5th axis. See settings 30, 34 and 48 for the 4th axis
and 78, 79 and 80 for the 5th axis.
Setting 85 should be set to .0500 for 5-axis cutting. Settings lower than .0500 will move the machine closer to
an exact stop and cause uneven motion.
G187 can also be used in the program to slow the axes down"

MC

Click to expand...