[Matt@RFR]

Hey guys, I'm about to use my HRT160 for the first time, and I have a couple questions. This is a new rotary table in a new VF-2ss that's wired for the 4th.

What is the maximum travel in degrees? On the Haas website, it sais 999.999º/step, but what does that mean exactly? The posted code for my part has it traveling to -6364851º! Will I have to break up the code and unwind the 4th every so often?

The other thing I can't find is the max feedrate for the 4th. This part has a 3/32" ball nose making a sharp point at Z0 at 60ipm, so the feedrates that are spit out by Mastercam are up in the 2000 area.

[Geof]

.....What is the maximum travel in degrees? On the Haas website, it sais 999.999º/step, but what does that mean exactly? The posted code for my part has it traveling to -6364851º! Will I have to break up the code and unwind the 4th every so often?....

There is no maximum travel as far as I have found; you can just keep going round and round.

To avoid having to 'unwrap' by the same number of degrees to take the Rotary home you have to turn on Quick Rotary G28 and CIRCLE WRAP.

Setting #108 is Quick Rotary G28.

CIRCLE WRAP is one of the items under PARAMETER 43, put a 1 here.

Depending on the age of your machine you may find that CIRCLE WRAP is a Setting not a Parameter.

[Matt@RFR]

Thanks Geof!

[crazymat14]

Geof,
Will this work on a TRT-160 trunnion style for the B axis?

Matt Gifford
Neal Chance Racing Converters

[chmillman]

What I found on my 1999 machine (maybe they have changed this by now) was that with programming it quit at about +/- 200,000 degrees. however, if you advanced it by programming more than about 100,000 degrees, if you then put it into manual, the handwheel would no longer work.

My feeling is that an operation in excess of 6 million degrees may be risky, so you may need to break it into sections.

The max feedrates for each Haas 4th axis model are specified on their website, every one is different. They are in degrees per min, so you will need to convert degrees of rotation into a linear measurement based on the diameter you're milling. You need to enter an "average" 4th axis diameter in the control (I forget what setting) in order for it to calculate the rotary feedrate. --ch

[Geof]

......My feeling is that an operation in excess of 6 million degrees may be risky, so you may need to break it into sections......

Would G92 work here? Rotate the table a few hundred thousand degrees then use G92 to define the current position as A0.0 and continue cranking?

Then use G28 with the Quick Rotary turned on to get back to a known zero.

[Matt@RFR]

I haven't got far enough to worry about the max revolutions yet, I'm still stuck on the feedrate thing. On the Haas website, it sais 100º/sec, so 6000º/min. BUT, in MDI, the max feedrate I can put in is 833, which just happens to be the max X and Y feedrates. Is there any settings or parameters that I'm not finding that control what type of feedrate the 4th excepts? Or a G/M code to set a condition??

The problem is that I'm working on a christmas present for my wife, and this is the first time I've used a 4th axis. My CAM program is outputting the feed as degrees per minute, and it's alarming out. I don't get it.

[chmillman]

No, the Haas wants IPM or MMPM, not deg/sec.

It uses the diameter setting (again, I forget which number it it) to calculate the degrees per second from the IPM/MMPM given. --ch

[Matt@RFR]

Looks like I'm screwed then. Mastercam refuses to post anything other than degrees per minute feedrates for the 4th. Great. And this program is in excess of 600,000 lines, the majority of which have 4th axis feedrates.

Thanks for the help anyway.

[Donkey Hotey]

Uhhh...believe me, I'm no expert on MasterCam or the rotary (in fact, I'm just smart enough to be dangerous) but...

...I think it's just a matter of doing some math in the post processor. MasterCam outputs 'units'. The postprocessor decides what to do with those units. I think that you can find that portion of your post, add some math and convert it to IPM.

In any case, I'm paying particular attention to your results. I have a T5C rotary that has never been connected to my VF-2. I have factory 4th axis and the outboard control for the 5th. I'm going to have to cross this bridge soon.

[HuFlungDung]

If you insert a diameter value in your Haas settings for your HRT160, the control will convert your IPM as required. Of course, this implies that you are working at more or less one diameter on the entire job, because you cannot change the settings midway (easily).

So, if you have a proper X or Z feedrate specified for the tool, there is no actual need to specify an A axis feedrate, because the A axis will move at a comparable feedrate as the last linear axis feedrate (thank god, on a Haas ) If you have a combined XA move, the linear feedrate is 'boss' anyways, and feedrate is modal and does not need to be declared on every line unless you wish to change it.

Now the above may be just a workaround if you cannot find a way to easily modify your post, but heck, you gotta get that job done in just a few hours

[Matt@RFR]

Donkey's post got me thinking, so I had a look at the post processor, and just to see, I forced it to use inverse feedrates for the 4th, then reposted the code, and walla, everything is 833ipm or less. Even if it's too fast, I'll just override the feedrate until it looks ok and sounds ok. Cross your fingers!

Attached is a picture of the model I'm trying to make. It's a lighthouse of my own design, based loosely on my wife's favorite lighthouse. It is about 8" tall and I'm starting with 5" square bar.

[Donkey Hotey]

Hey guys, I'm about to use my HRT160 for the first time

Nothing like stepping into 4th axis with something easy, huh?

I want to see pictures if you manage to get it to work.

Have you thought of doing a roughing program to get it down close to net shape and a second one to just remove the last 0.050"? 600K lines sounds like a lot of code.

I would imagine you're under some stress to get this done before tomorrow, huh? Good luck with it. I'd like to see some pictures of it in process and when it's done.:cheers:

[Matt@RFR]

Nothing like stepping into 4th axis with something easy, huh?

That's pretty much my M.O. I bought the mill with zero CNC experience too.

As for roughing, your idea is exactly what I did. I roughed it with a 1/2" endmill to .050" of the finished surface, and am now running a 1/2" ball nose within .015", stepping over .050". The finish tool is a 3/32" ball nose at a .002" step.

The inverse feed thing worked great, but the 1/2" ball nose has seriously gouged the part, scrapping $200 of mat'l and probably 100 hours of my time. I have no idea what went wrong, but I'm gonna go ahead and finish it since it's in the machine, just to see what else goes wrong so maybe I can learn a little. I'll post pictures when I chear up. Man, what a downer.

[Donkey Hotey]

Wow, bummer on the botched toolpath.

$200 worth of material? Aluminum? I see you're in Paradise. Are there any decent industrial metal places in Sac?

Industrial Metals here in So Cal gets $1.69-1.89/lb for aluminum 'scraps'. Their scraps are usually a heck of a lot bigger than the bar you used.

My math puts that bar at about $40. For that kind of cabbage, you could even afford the gas to drive to Sacramento & back.

Just an idea for when you run the second take on it.

And we're in the same place with the machines: my VF-2 is also my first CNC. Big learning curve to do by yourself. It's good to have found this place.

How did Mastercam do with the preview? I've had problems with the simulation doing things differently than when they get to the machine. Frustrating.

Looking forward to your next update.

[vanmjim]

looking for a good used HRT160 with servo
new combo is apx 9300
Does anyone have one available around 4500
jim