Feed for A axis is different

[Lathe-Mill]

I just like to know if there is a way to fix this little problem, okuma mill, the A axis feeds on IPD (inches per degree), Z axis on IPM (inches per minute).

the part I am trying to machine has all types of fillets and angles and it is using all 4 axis at the same time : X2.00 Y.50 Z1.75 A2.0 F200.

with that feed rate there , the Z axis will move at 200 IPM, but it's the right feed for the A axis.

feeding at 200 ipm on the Z axis will damage the part and probably the tool.

any sugestions will be appreciated.

thanx .

[5 AX]

In order to cut the part you will need to use inverse feed time (g93).

[Lathe-Mill]

jesse, thanx for your reply; but i am not familiar with the G93 code, also okuma mill wont support it, i looked in the manual and there is nothing about it.

could you please explained what that code will do? thanx.

[Guest CNC Apps Guy 1]

Quoted from Modern Machine Shop Online

Here Online Supplement - Postprocessor Considerations In Multi-Axis Machining

 

quote:

---

Most NC programmers think of the F-register in a CNC controller as the method for specifying linear velocity, i.e. uPM or uPR. This is true for two- and three-axis linear motion, but when rotary motion is to be controlled, the F-register takes on a different meaning. When combined linear/rotary motion exists, most good CNC controllers require the inverse of the amount of time necessary to make the move, and since each move has a different distance, the corresponding time varies for each block as well. The exact reasoning behind using the inverse value rather than the direct time in minutes or seconds is simply a historical matter.

 

Calculating the F-Code

The constant used to calculate the inverse time code is normally 1 minute, such that the equation is:

 

F(code) = 1(minute) / (time = 3D distance/velocity)

The 3D distance of the move is calculated in model coordinate space at the NC control point, not in machine coordinate space and not necessarily at the tool tip. For example, a 5-inch move at 50 IPM takes 5 50ths of a minute, yielding an inverse time calculation of 1/.1 and an F-code of F10. The same 5-inch move at 700 IPM would be 1(minute) / (time = 5 / 700) or (1/(5/700)) or (1/.0071428) or F1400.168

 

Variations To The Equation

If this value exceeds the F-Register format, the common reaction of a postprocessor is to output the maximum value of the F-register (F999.99 if the F-register format is 3.2), a signal to the part programmer that a problem exists. When this happens the CNC machine does not achieve the programmed velocity, and unless the F-register can be re-assigned, the machine simply cannot process the move(s) faster.

 

Since the typical CNC's F-register has a 3.2 or at most a 3.3 format, the need obviously exists for some way of controlling the results of the equation to avoid "over-stuffing" the F-register. If the machine normally operates at a high (over 500-1000 uPM) velocity, the machine tool builder sometimes changes the interpretation of the numerator in the inverse time equation to 1(second), or in extreme cases 1(millisecond). When the numerator is 1 second the above F1400.168 would then be coded as 1 / (time = 5 / (700/60)), or F23.333.

 

Invoking Inverse Time Mode

Most CNC controllers equipped with inverse time require a G93 to declare the feed mode on the initial move containing rotary motion. The general rule is: If a G93 is required to invoke inverse time mode, a G94 or G95 is also required to cancel it. This means the first of a sequence of normal XYZ linear moves with no rotary A/B/C word(s) will require a G94 and an F that is interpreted in uPM.

 

Most controllers that support G93 inverse time require an F-code on every move, even if it does not change from the previously programmed value. A "feed hold" will occur if this rule is violated. This situation normally happens when machining a cylindrical or spherical surface since the chordal moves are of equal distance and the velocity is constant. There is a spec setting that forces redundant F-codes for inverse time which should be set unless it is specifically known that the F-register is modal.

 

Poor Man's Inverse Time Feed

Because inverse time calculations can appear confusing for the uninitiated five-axis programmers, some machine builders have attempted to simplify five-axis programming by offering a form of "poor man's" rotary feed control where the CNC operator manually sets the fourth and fifth axis radius values.

 

This type of feed control can work well for machining simplistic cylindrical or spherical shapes, but since the tool tip is normally in a state of constant change relative to the center of each rotational axis when in five-axis contouring mode (especially true when machining doubly curved surfaces), the true tool tip velocity is never truly maintained.

 

A good post will automatically generate inverse time feed calculations, and you can scale the F register to achieve minute-based or second-based calculations.

---

Hope that helps.

[steve f]

T@T@LO.

 

I think you have invented a new type of feed (inches per degree) or maybe you just meant DPM (degrees per minute) or I'm clueless. An inverse feed value is used to specify motion between points within a set amount of time instead of at a specified rate of motion. The F value in inverse feed is actual a number that 1 is divided by to come up with a time value within which the machine must execute it's motion. The reason inverse instead of actual time values are used is so that the operator doesn't have to switch their thinking about feed rates and just specifies a higher value if they want higher feed.

 

HTH

 

steve

[steve f]

Damn...I'm always two seconds too late.

 

steve

[Lathe-Mill]

Thanx James, it's very informative, i understand a bit more, now all i need to do is see if i can get the post to do that.

[Lathe-Mill]

lol..

steve, thanx for you replay, like i said , i never worked with G93 and the okuma mill doesn't have that option (according to the book)..now i am trying to get someone from okuma so i may get this going, I appreciate all you guys replays, tahnx!

[md]

In inch system it is posible to specify how

the F (F = 1) value will be interpeted as

1 deg./min or as 25.4 deg./min.Change bit 7

of *NC OPTIONAL PARAMETER*(bit)No. 15 to 1

F10(10 deg./min) realy is *254 deg./min*

It WILL NOT change inch/min.

[Brendan P]

James...

Reading that just gave me a migraine.

Wayyyyy too heavy for meeeee.....

[crazy^millman]

Is this a indexer that is an add on wit ha seprtate controller by chance. If it is then you may have to do what I did at one place and that is play the wait code game. I made soem rool cams on a machine with a seprate controller not fun. If the machine is a indexer instead of a full 4th axis this could also be why yuo can get the sync you are looking for. If not then look through what was said and see if by doing what was said you can get the z axis to sync with the A axis I think that will be your best bet verse trying to go the other route. Good luck let us know what you coem up with.

 

 

Crazy Millman

[Lathe-Mill]

okey guys, here is what it was explained to me by the okuma applications dept.

he said that mastercam will convert that feed rate to d.p.m, the feed rate you see in your control it is actually feeding degrees per minute.

i was nervous cause the control was giving us an alarm, something like "feed rate was over the maximun feed rate", i cant remember the exact phrase.

so when i saw X , Z , A , F300. plus the alarm, wow , we panic.

we thoughed was i.p.m

when i input a feed rate on my parameters like 10 , it posts like 250 +/-, wich it is d.p.m

 

THANX TO ALL FOR ALL YOUR HELP!!!!

[crazy^millman]

Cool Beans and where is your avatar.

 

Crazy Millman

[Lathe-Mill]

no clue locomillman

how i do that?

[Brendan P]

quote:

---

Cool Beans and where is your avatar.

---

funny mill man,i just asked him the same question in another thread.

 

Juan,get a pic. of you choice and send it to Dave the Webby.

It needs to be "sized" first.

He should be able to help you.

 

 

Where's yours millman????

[Lathe-Mill]

thanx bucket

[crazy^millman]

Still have not find that right one yet give me time I will come up with a good one Bucket.

 

 

Crazy Millman

[chris m]

Juan

 

Glad Morris helped you out. Was it Bob; or somebody else? They are pretty good guys over there.

 

C

[Lathe-Mill]

was bob baldizi, great guy.

[Lathe-Mill]

could someone tell me how to e-mail someone here in the forum?.

thanx

[Brendan P]

Aaahhh....

You would first have to tell us who you want to Email..

We are not mind readers! J/K

there is an icon on the post of the person you want to email.

It is they're profile.

Click on it,and if they have their settings on,it will have an email add.

Or you may have to Email them thru the board.

[Guest CNC Apps Guy 1]

See the litle envelope looking icon next to someon's name? Click that and it gives you the person'e e-mail addy. Then you can click on the e-mail addy and your default e-mail editor shoudl pop up, and yadda, yadda, yadda.

 

HTH

[Lathe-Mill]

i selected in my profile not to show my e-mail, but i got 3 e-mails, how they did it?

how to do it thru the forum?

[Jean-Simon]

When you select not to show your e-mail means people won't know your address but will still be able to e-mail you, you need to select " No, hide my address and do not allow members to mail me " HTH!

 

Simon

[chris m]

The Robert E. Morris Company ROCKS!

 

Shameless plug as my shop is basically an Okuma showroom

 

C