Max G94 feed?

[extanker59]

We are trying to fine tune our CAM post to use inverse time feed. In some instances it will post a really high feed in G94. They all look huge but some are much bigger. This one stopped the machine. What should I tell the post writer is the max?

X.9109 A17151.831 F3560.1936
A17154.791 F3340.2802
A17154.881 F110808.8799
X.911 A17157.675 F3538.2121
A17159.706 F4867.7878

Also, should the feed have 4 decimal places?
I always assume the post writing guys know more but...?


We're having a heck of a time getting the full 4th axis programming going. The motions are jerky at non-inverse time G94 IPM feed rates over 24 with pseudo dia [setting 34] set at .2 (the average diameter of these parts).
G93 is just as bad so far.

Haas VM-2 with HA5C rotary, High speed machining on.

Thanks
Chris

[Delw]

chris,
I always thought g94 was a rapid feed? when I use it on my omniturns I dont have any decimals over the max rapid. Matter of fact never tried decimals.

as far as the jerky motion thats usually cause by running small segments and NOT having the highspeed turned on. if its in g94 feed maybe thats too fast? try it in g95 which is usually a feed rate.
Also maybe there is a setting for the jerky motion ( I forget the name) but geof has touched on it a few times, its like semi finish rough finish etc etc.

I use g01 for my feed on my full 4th axis

Delw

[extanker59]

G93 is Inverse Time Feed Mode On
G94 is Feed Per Minute On (Inverse off)

I am using G01, just in G93 mode.
Haas mills must have a maximum feed rate in G93 mode. I can't find it in the book.

What about the decimals. Another answer said he uses 2 so I'll do the same. Four places did seem silly.

Here is what the Haas answer man said about G93:

"This VMC/HMC feature specifies that all F (feedrate) values are to be interpreted as “strokes per minute.” This is equivalent to saying that the F code value, when DIVIDED INTO 60, is the number of seconds that the motion should take to complete. G93 is generally used in 5-axis work, and sometimes in 4-axis work as well. It’s a way of translating the linear (inches/min) feedrate assigned to the program – F30, say – into a value that takes rotary motion into account. When G93 is activated, the F value will tell you how many times per minute the stroke (tool move) can be repeated, based on the linear F value.

Haas has been able to accommodate full 5-axis machining for many years; however, this feature, in conjunction with aftermarket CAM systems and their post-processors, offers even more flexibility and versatility."

[Delw]

right but your feeding it at F110808.8799 IPM thats flat out fly'ing if your machine rapids at a max of 1200 IPM

[extanker59]

"but your feeding it at F110808.8799 IPM "
No, no, its feeding so that it takes .00054 seconds to make the rotary move .09 degrees. G93 is strokes per minute according to the definition provided by the Haas answer man.
Not as fast as it looks.

[Delw]

Ah ok, now I understand. Sorry for the confusion.
I use g01 feed for my rotary however I have noticed I have to change the feeds for certain Dia's.
I usually just made it work and let it go, never really thinking about it.

[underthetire]

There is a setting for diameter for the 4th axis. Have you played with that at all? I'm curious as I just put our 4th on but havnt run the machine yet.

[extanker59]

I am using that setting now to approximate a mean diameter but I have some parts that vary in diameter a lot so I'm trying to use G93 to take that into account.

It works fine as long as your cut diameter stays in that area. Just have to be aware of that setting and change it for the different parts you set up.

[KenFoulks]

Anytime a customer has jerky motion, the first suspect is parameters. Email your parameters, settings, and program with a picture or description of your part to Apps@haascnc.com and we can run a parameter-check program.

With high speed machining turned on, the max feed is 43000 for Inverse Time (G93).

When using Inverse Time (G93) the value of setting 34 has no effect. Feed per Minute (G94) is affected by setting 34.

You can output 4 decimal place feed values, but 2 is sufficient.

[extanker59]

Thanks Ken. Already had a tech out and he verified the parameters. He also copied everything else as well as the program and was going to send it to California. This was late last week. No response yet.