New VF 4 SS w/TR160

[makingchips]

Hello again everyone. The company I work for just purchased a new VF4 SS with the TR160 4th and 5th axis. Here is my question. I'm comming from a Fadal 4020 with the TR 4th and 5th axis, I'm using X3 for programming. With the Fadal you had to set the tools to the center of the axis rotation (6.xxx) then have the part and fixture offset the differance in MC from that point to bottom of the fixture (6.477) to get it to make parts.

Will this be the same on the Haas or can I set the tools to the top of my fixture on the platter and have the part/fixture bottom Z0 in mastercam? It does not have the tool setter, it will have to be done manualy. We are waiting until Tuesday 12/2 for the Haas guy to come up and finish the install, until then we cant power it up. It came in the door 11/24. It has been sitting there begging me to run her, so naturaly I have had time for thinking and is why I'm posting this question.

I have pic's but have to make them smaller to post.

Chips

[makingchips]

[Donkey Hotey]

I'll be interested to hear from any other 5-axis users but this is my take:

The Haas only addresses the axes numerically (distance XYZ and rotation AB). It doesn't do any magical conversions for you. This is more of a Mastercam question than a Haas question but I don't think it's going to be any different than the Fadal.

I had to get my brain around 5-axis programming and how you'd handle offsets. Using the center of rotation is the only way that makes any sense to me. I'm curious to learn anything you've got to share (I have a T-5C rotary but I don't have a 5-axis license for my seat of X2).

[makingchips]

Originally Posted by Donkey Hotey I'll be interested to hear from any other 5-axis users but this is my take: The Haas only addresses the axes numerically (distance XYZ and rotation AB). It doesn't do any magical conversions for you. This is more of a Mastercam question than a Haas question but I don't think it's going to be any different than the Fadal. I had to get my brain around 5-axis programming and how you'd handle offsets. Using the center of rotation is the only way that makes any sense to me. I'm curious to learn anything you've got to share (I have a T-5C rotary but I don't have a 5-axis license for my seat of X2).

What no magical conversions button on the new machine. I hope it is equipted with the magical just push the green button and it reads your mind and makes the part. I was actualy asked on Wednesday how long it will be until I'm up and making parts. BTW I have the easy button from staples so I should be ok. lol

All the programs I make with X3 are live 5. Anything I can help you with in programming of 5 axis I will be happy to share once I learn it on the Haas.

MC

[Donkey Hotey]

When I got started with this, I wondered if it had some transformational positioning so that it knew the model of the rotary and could park a cutter tip at the center of the mounting face and translate around that spot. No such luck. It's all got to be done in the CAM system.

I didn't get full 5-axis wiring with my machine so I didn't get full 5th in Mastercam either. My rotary has never been hooked to the machine (4 years). One of these days, I need to get around to doing that.

[slatern44]

What options did you get with this machine? it looks pretty loaded.

[makingchips]

30 hp 12000 rpm direct drive spindle.

1.2 second tool changer.

programmable coolant nozzel.

Auto air blast.

300 psi thru the spindle coolant, cutting mostly graphite so no need for the 1000 psi.

Glass scales on XYZ.

1400 IPM rapids, 800 ipm cutting.

Auto doors.

coolant filter.

chip auger.

high intensity lighting.

16 MB of memory.

USB port.

TR 160 5XB wired directly to the machine (not in pic)

That is all I can think of right now.

MC

[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.

[makingchips]

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.

The Haas tech is comming in on Tuesday set up and finalize the machine install. I know I was told I have to put the trunnion table on after he does the 3 axis set up verifacation, then he will set up and verify the trunnion table. I have to mount it to the machine for liability purposes.

So basically what you are saying is use an indicator touch off the table zero the indacator move up touch off the platter at horizontal. Now if this is correct do I use this number in master cam or do I add it to the tool on the machine? On the fadal it was both because on Fadal trunnion tables the platter is above the B (tilt) axis rotation unlike the Haas. On the fadal I ended up with something like tool tip Machine z at 7.(table to center line rotation) and in master cam 6.477(center line rotation to platter) from Z 0 for a total height of 13.477 between the machine Z and Mastercam Z.

Will the tech set up parameter 85 and the backlash?

Thank you.

MC

[DRD]

Mastercam programs off 0 as a datum, or referance. Ther machine is referanced, x,y,z,a,b, just as it referanced in mastercam.

The easy way is to measure the true diamater of trunion OD of the platter, then devide by 2, the will give you the center measurment of the plater, take a measurement from the top of the haas table, to the top of the plater, flipped 90 degress on it side, then subtract 1/2, and there is your true center line, and Z zero offset.

You can use the touch probe maually, with a mdi, m53 to turn on the probe, touch off the haas table, and use the origin, to zero out the Z axis indicator, now move the probe over to the fliped 90 degree A axis trunion, table, and touch off the top on the center of the table, enter this value in the offset, and subtract the 1/2 of the diamater, and enter this value in the offset, this is your new z offset, A center line. No your machine is aligined with mastercam.
Remember, that all the offsets on the haas are in machine cordinates. I use a tool presetter, so all the tool lenghts are taken care off, and the G43 takes care of the tool lenghts in the maching process.


Most likely, the tech will know nill about the paramter 85, it's in the book, and backlash, these are items the end used fiqures out. Hass has put in the back lash at the factory, but they may need some tweaking. The Haas is a nice machine, but needs fine tunning by the user, the HFO are clueless about 5 axis stuff. You will soon know more, than HFO techs.

[makingchips]

Thank you DRD.

MC

[makingchips]

On a side note I plan on setting X,Y,0 on the 1.5 dia. center hole on the platter. Then mount my tooling plate I made to the platter with a 1.4995 pin I ground. All the fixtures I use will mount to the tooling plate located with 1/4 dowel pins and 1/4-20 socket head cap screws. I allways program to the fixture center in X3. The pins on the tooling plate makes sure my fixture is located on the machine X,Y,0 that is on the platter. This method worked great on the fadal, I hope it works as well on the Haas.

MC