going from vf3 to vf4ss

hello,
we are trading in our 10 year old vf3 for the vf4ss. i have never dealt with the side mount tool changer, so will there be any difference as far as programming and does it
keep the tool in the same pocket all the time?
and, it has high speed machining option, is there a g code for that??
any other differences??

thanks much

You can call the next tool with a side mount. example -
t1 m6
g0 g90 g54 x0. y0. s3500 m3
g43 h1 z5. t2
Just make sure the next tool call is after the g43 (if you have H&T code agreement on, which I highly recommend).
This will call up tool 2 and move the carousel so that it is ready to swap out when you are done with tool 1.

The pockets constantly change the tools since they are swapped, i.e. in the example tool 1 would be placed in the pocket that tool 2 was in. So pocket 10 had tool 2 in it, but now it has tool 1 in it. You can also call tools by the pocket number in mdi, comes in handy for unloading tools or if you don't know what tool number that face mill is off hand.
Don't think there is a gcode for HSM, but there is a G187 P1(2)(3) to call out default finishes, also you can call an E value for corner rounding, example -

G187 P1 E.05 would be a roughing mode (P1) with a max .05" corner rounding (E.05)
G187 P3 E.005 would be finishing mode (P3) with a max corner round of .005" (E.005)

so tool 1 is always tool 1 no matter what pocket number it in?

chineshop_guy said:

so tool 1 is always tool 1 no matter what pocket number it in?

Click to expand...

This is correct.

VAs stated already, tool 1 is always tool one and so on, but its carousel pocket designation will constantly change. And in case you were wondering, no this feature cannot be changed nor would you want it to.

I always tell people not to worry about where it is at in the carousel, just call up the tool you want like you are used to; T10 ATC FWD/REV done!

There is a screen display that will show you what pocket a particuar tool is located in at any given time.

Because you have a side mount and it's an SS machine, look up oversized and heavy tools in your manual and fully understand how and when to label a tool as such. Heavy and oversized tools will need to be flagged prevent potential machine and/or tool damage.

Enjoy the new machine!!

There are a few things to learn with the side mount, but you will love the speed and ease of use quickly. A much much better tool changer hands down!!

BTW, is the VF-4SS a new or used machine? If new, the tech setting it up for you will go over all of this and much more.

Mike1974 said:

You can call the next tool with a side mount. example -
t1 m6
g0 g90 g54 x0. y0. s3500 m3
g43 h1 z5. t2
Just make sure the next tool call is after the g43 (if you have H&T code agreement on, which I highly recommend).

Click to expand...

How come after g43? I have h&t agreement on and ive been putting the next tool call up before g43, the next line after tool change actually. Will this get me into trouble? We've had our new haas for a few weeks so im still getting used to these little things.

Kapster said:

How come after g43? I have h&t agreement on and ive been putting the next tool call up before g43, the next line after tool change actually. Will this get me into trouble? We've had our new haas for a few weeks so im still getting used to these little things.

Click to expand...

I am not 100% sure, but if you don't have it called out correctly in the program the H&T code agreement alarm will go off and stop the machine. If I understand you are doing something like this -
T1M6
T2
G43H1Z5.
I think that should trigger the alarm because you have called T2 but then used H1 ...? It could vary by how new the control is also. Maybe now the T number is tied to the M06 command so how you have it is not flagging the H&T code alarm? Maybe a Haas tech can weigh in on this.... But I would say if your setting is indeed on then I wouldn't worry too much, unless that setting is "broke" somehow! Can you post a bit of code here?

Ok I answered my own question. I ran a short MDI as above with the next tool called (to get it ready in the carousel) before the G43 offset and it was fine. Upon closer inspection, I used the help function (new machine, only a couple months old) and it says for H&T code agreement on - "the machine checks to make sure the H offset matches the tool in the spindle". I am pretty sure this is new, or it works slightly different than some older machines as I remember seeing it alarm out before... A nice improvement to the software!

You can stage tools wherever you want to. Most posts (or normal posts) seem to put it on the G43 line.

G187 is on pretty much all Haas machines so you are probably already familiar with it. It will work exactly the same on the SS or non SS machines and also on machines with or without High speed machining. High speed machining allows a higher max feedrate and further code look-ahead.

Yea thats exactly what im doing, must be something they changed then.