G93 question

[Chap54]

Hi all,

 

I'm working on trying to learn 5th axis programming. We have come up with some programs we are trying out using the G93 function. What is the relation between the feed rate I choose in mastercam  and all the feed rates posted out in the g code, if any. The first time I picked a feed rate of 5 ipm to post, and it was ridiculously slow. So I re-posted with a feed rate of 100 ipm, and it is still to slow. Is there any rule of thumb to go by when choosing a feed rate in mastercam?

 

Thanks,  DC

[Guest MTB Technical Services]

Unit per Minute Feedrate values are for linear axes.

This type of feedrate doesn't apply to rotary axes.

The common element between the two is time.

 

Inverse time allows you to specify a feed value for a move based on time.

This guarantees that all 5 axes will arrive at the endpoint at the same time.

 

Inverse Time Feed = 1 / (3D Length of Move at Tip of Tool /Unit per Minute Feedrate)

 

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.

Larger values indicate very small moves.

Small values indicate large moves.

 

All of this is handled by the post-processor.

You would still enter the UPM feedrate in any operation field in MC.

 

http://www.mtbtech.net/blog/2012/11/24/5-Axis-Machining-Demystified-Part-Three.aspx

(Near the bottom of the article)

[Guest]

Can also chew on this...

 

http://www.eng-tips.com/viewthread.cfm?qid=200454

[Chap54]

"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."

 

This is going to take a while to digest. I understand the the F rate takes on a whole new meaning, but I need to wrap my head around what is actually happening between my computer and the machine. All my programming experience to this point has 3 axis. When I change the feed rate inside mastercam, on the

page you set tools feed & speed- regardless of what number I put in there, I max out at F1000. when posted out. Am I correct in assuming that I have

some other problem based on the 2 paragraphs quoted above? In running the program on the machine, we have to use "dry run" mode just to get it to run at what looks like would be correct.

[Guest]

Other than over thinking it, you can set your posts maximum value to match your machines ability....

 

You're going to have to find out in the manual likely what the fastest your machine can move, then set your post to max out at that.....you will set your feederate and the post will handle the feed output

[Guest MTB Technical Services]

FANUC typically supports 5.4 for the F address.

I have never had an inssue with Inverse Time on FANUC controlled machine.

 

Don't need it as much anymore as the newer controls support TCP.

[civiceg]

TCP is only for 5 axis correct?

[djstedman]

If you get a Max value of 1000.00 when posting .. I would suggest that the next thing you do is simply modify that value at the machine to a higher value.. make it 2000.. then try it.. does the machine alarm out? Keep trying values until the machine alarms out and you can find your actual Max for F  (I would strongly suggest running in the air when testing this..)

 

If 1000.00 is the actual Maximum.. then I would say you need to talk to the people you deal with for your Machine and see if there is a parameter or something that can be changed to modify the time settings.. If you find the value can actually go to 9999.99 or 99999.999 (or any other value) then the solution is to modify Inverse Time Feed Rate Limits in your General Machine Parameters in your Machine Defintiion to use the new maximum F value you figured out..

 

I realized after posting this.. that I probably should have stated that the 'correct' thing to do would be to look up the proper values in the manuals / documentation.. I have found in practice however that the documentation is generally pretty hard to find for this stuff.. and that's if the shop has kept track of all manuals and documentation to begin with..

[Guest]

I avoid INverse Feed like the plague. TCP is THE way to go. :

[Guest MTB Technical Services]

TCP is only for 5 axis correct?

 

No, It also applies to 4-Axis.

 

I mean full 4-axis, not an axis substitution with an additional rotary axis output.

 

On FANUC, G93 isn't needed with TCP  as TCP only supports G94 UPM.

In fact, it will generate an error if you try it.

With TCP, the control itself figures out the correct rotary velocity, for the given UPM, to get simultaneous rotary/linear arrival at the endpoint.

[Thee Awbade™]

No, It also applies to 4-Axis.

 

I mean full 4-axis, not an axis substitution with an additional rotary axis output.

 

On FANUC, G93 isn't needed with TCP  as TCP only supports G94 UPM.

In fact, it will generate an error if you try it.

With TCP, the control itself figures out the correct rotary velocity, for the given UPM, to get simultaneous rotary/linear arrival at the endpoint.

 

 

I had no idea my TCP was doing this. Learn something new every day. 

 

TCP Is a pretty fascinatingly cool function 

[JMahon]

My posts have always done inverse time. I got a part I'm gonna try TCP on tomorrow.

So TCP is technically more accurate?

[civiceg]

So what would be favored on a true 4th machine? Any cost difference between options on a Fanuc?

[Guest MTB Technical Services]

My posts have always done inverse time. I got a part I'm gonna try TCP on tomorrow.

So TCP is technically more accurate?

 

 

No. Accuracy is not increased by using TCP.

It simply eliminates the need to worry about the gage length of tools when using a profiling head.

TCP also maintains the relationship of the tool center point or tool tip (depending on how you use it) to the workpiece.

Without TCP you would be programming the center of rotation as the control point.

 

 

 

Without TCP

The rotary command A90.0 causes a movement of axis A without any linear axis movements that would keep the tool in contact with the part.

 

 

With TCP

If TCP is active, the same command causes the swing of 90° with displacements of the linear axes to maintain the tool tip at the same location.

 

 

 

 

When using TCP on a dual-rotary table/table 5-axis, TCP can help minimize the travel within the machine envelope.

However, you need to be careful under this circumstance as you can easily have a situation where one rotary reaches max velocity almost instantly.

In these cases you need to make sure you have plenty of look-ahead and also have the smoothing option.

You should get those anyway as they only make sense for 5-axis but they aren't required.

 

When TCP on a FANUC is called with the smoothing the code looks like this.

 

G43.4 P3 H?? X.... Y... Z.... A... B...