G08/G09 usage

[Cole2534]

G-Coder mentioned this in another thread but I've had the question for a while. I don't really understand when to use one or the other. My CAM (F360) defaults to G9 and this is what I've always run.

Could someone give an instance of when no acceleration would be needed?

 

[Delw]

On my fadals I always use a G8 , then g9 to cancel since the beginning. if I need to slow the feeds down I do it when programming.
in the 30+ years I been running machines there has only been one instance to where I needed to use the code. I didnt even know that there was a code for it until I got a program from my customer that had it alread in there. I deleted them out ran the part and it was kinda funky. one day I asked what that code was and he told me. next time I got the job I ran it and the parts were perfect. I believe it had to do with exact stop or something like that.
my parts are supper thin and most corner rads are + or - .005 on small corners rads as well as deep this one in particular was + or - .0025 using a 3/32 endmill.

on a fadal it does help if you have any slop in the machine on the bigger rads. but if your machine is tight and doing even tighter work then it helps alot

 

[Delw]

I'll try to find the code, it isnt a g8 persay there is a code with a .1 after the g code.

 

[Herding Cats]

I know nothing about Fadals but will take a jab.

On a Fanuc G9 and G61 are exact stop mode when the machine will completely execute a block before proceeding to the next, ie. it will leave a very sharp outside corner. On a Fanuc G64 is cutting mode and G62 is corner override where it will slow down a predetermined amount for arcs smaller than a specified radius. Also on Fanuc G8 is either lookahead or accel/deccel BEFORE interpolation, similar to G5.1 and G5.

Maybe some of this is useful with Fadal......maybe not

 

[Cole2534]

I mill some round bosses, 1.000, and they come out usually a little over maybe .002 at most but it leaves witness marks where the code changes.

Would G08 prevent this? in this case aesthetics would be preferred over accuracy to an extent.

 

[Delw]

yes kinda fadals are notorious for leaving witness marks due to many things. tool pressure tightness of machine etc.
slow your feed rate way down and use a lead in and lead out. all my dias I use a dry pass one never lifting the tool and use a feed out as well.

 

[Delw]

Cats
I'm not technical on stuff like that but heres some info on the fadals. you can probably decifer better. I believe my program was the g51.2 that was used.

G51.2

Tool Load Compensation State Feed Rate Before the G51.2 Line R1= Target Spindle Load R2= Min. Percentage Feed Rate Reduction R3= Max. Percentage Feed Rate Increase R4= Time at Min. Feed Rate to Initiate Slide Hold

as well as this one

G91.1	High Speed Execution (-2 System Only)
G91.2	High Speed Execution Cancel

 

[Herding Cats]

Cats
I'm not technical on stuff like that but heres some info on the fadals. you can probably decifer better. I believe my program was the g51.2 that was used.

G51.2

Tool Load Compensation State Feed Rate Before the G51.2 Line R1= Target Spindle Load R2= Min. Percentage Feed Rate Reduction R3= Max. Percentage Feed Rate Increase R4= Time at Min. Feed Rate to Initiate Slide Hold

as well as this one

G91.1	High Speed Execution (-2 System Only)
G91.2	High Speed Execution Cancel

If I had to take a wild off the wall guess I would say R2 and R3 are time constants for Deccel and Accel by way of percentage. Fanuc parameters are based off off ms as well as allowable speed differences

 

[g-coder05]

On the 3016 I was running the G8 was “precision cornering”. I was doing some pocketing on electrical connectors and QC had me look at it on the optical comparator and it was like the tool drifted past the XY coordinate then tried to backtrack and correct it.

The best I figured is the deceleration was too hard. I finally found the G8 and tried it but you could see the machine actually pause in the corners. It became a toss up to either slow the feeds down on finish passes or use G8.

I don’t know enough about Fadal to mess with acceleration and deceleration to fumble with it so I just stuck it out.

 

[Delw]

when in G9 the machine for lack of a better term slams into corner than goes to next move all in one motion so to speak,.
when G8 is not active the machine goes to corner pauses then goes to next move.
I hope that I explained it well.
its kinda like the old machines at every corner they would pause for a split second before making that next move, I think the g8 so to speak at least for fadal was the highspeed machining deal they come up with in that tiome era.

 

[Delw]

Cole
do you know what dash number system you have on your fadal,?
mine is a dash-5 meaning the control was faster for processing (it was a low number but was upgraded before I bought it

 

[Cole2534]

Cole
do you know what dash number system you have on your fadal,?
mine is a dash-5 meaning the control was faster for processing (it was a low number but was upgraded before I bought it

I think it's a -4, but not sure which board to check to verify?

 

[Delw]

I believe -4 and 5 are pretty much the same as far as options and codes, Vanbiker might know.
Ive heard some people saying the g8 doesnt change anything but I believe those were the very early year options.
so essentially we have the same fadal control wise.

have you checked your mechanics to make sure everything is up to par ie backlash gib tightness thrust bearing play, as well as coupling fit.?
amp tunning is also a must and its really simple to due.
I did it with the following error display, when I had a tech in to do the ball bar test he did it with a mater and the following error display it was simple I hadnt done it in 2-3 years now.
the amps being tuned makes a huge difference in the way the machine runs it circles as well as angles. providing that the mechanics are all good.

your witness mark as you call it is more of a programming error or mechanics being off..
just remember with a fadal use a lead in, then g03 or what ever the dry pass then lead out with or with out comp and go at least 50% slower in feed on the circles. if you start training yourself to do that when programming it will minimize your witness marks or getting rid of them 100%.

almost every fadal should be able to run perfectly once the mechanics and tunning is done. tuning is free and easy, tighten gibbs is free and easy, the thrust bearings is pretty cheap ( i think 50 bucks a axis maybe 100) and kinda easy.
personally if you want a as perfect as you can fadal get it ball barred it ran me 500 bucks if I recall and money well spent. cause he fine tuned it , checked and tightened gibbs etc.

I believe I have pictures of all the stuff, basically just for my own reference when I was taking stuff apart, if you need them I can try to find them as well as help you out on it

Hope that helps.

 

[angelw]

As mentioned by others, G9 is an exact stop command, similar to G61. The difference is that G9 is valid only in the block its specified, whereas G61 is valid until cancelled by G62, G63, or G64. In both cases the tool is decelerated at the end point of a block, then an in–position check is made before the next block is executed.

G08 and G05.1 are used together. With the G08 function, the delay due to acceleration/deceleration and the delay in the servo system, which increase as the feed-rate becomes higher, can be suppressed resulting in specified values being followed accurately with errors in the machining profile reduced.

Regards,

Bill

 

[Delw]

Bill
I dont think the G05.1 is used that way on a fadal, according to the fadal book its used for a rapid.?

https://www.fadalcnc.com/media/pdf/tech_docs_1/User_Manual/Sect_2_M_Functions.pdf

https://www.fadalcnc.com/media/pdf/tech_docs_1/User_Manual/Sect_3_G_Codes.pdf

the m94.1 m94 .2 code added to a G8 code was the one I was thinking about that I said was a g91.1 g91.2 above from a customers program.
I'd copy and past them but they are long explanations and some have pics.

G8 Acceleration (No Feed Ramps)This code is used when no hesitation is desired between moves. If the toolhesitates the tool pressure lessens and the tool will leave a tool mark on thecontour. The G8 code would be used to eliminate the tool marks.The hesitation is called a feed ramp or acceleration-deceleration. Ramping isused to help the tool move to the desired position.

The G8 code is often used in combination with the M92 code.•This code is modal and will remain in effect until the G9 code is used.•The G8 code is a default code for format two.•The G8 code is incompatible with a G41 or G42 coded on the same line.•The G9 code is used to cancel the G8 code.EXAMPLE:G0 G8 G90 (Ramping is off at this line).G2 I.5 G91 Z.02 L7X-.5 G41X.55 Y-.55 I.55 G3•The M95 code is used as a non modal form of the G9 code. It is gener-ally used when G8 is in effect. See M95 for more details.

G9 Deceleration (Feed Ramps)This code is used when hesitation is desired between moves. When the toolhesitates the tool pressure lessens and the tool will leave a tool mark on thecontour. The G9 would be used to help the tool move from place to place wheninertia may be a problem. The use of the G9 code as opposed to using the G8code will help insure contouring accuracy.If an axis is faulting at a certain move, the G9 could be used to help themachine to get through the move by decelerating at the end of the move andthen accelerating again at the beginning of the next move.The deceleration will only slow the tool down at the end of the move. (It will notcome to a complete stop).•This code is modal and will remain in effect until the G8 code is used.•This code is default for format one.EXAMPLE:X1.0 G9X2.0X3.0G9 as an In-PositionCheckTo stop the tool completely at the end of each move, an in-position check mustbe used. The G9 code, used in succession on two or more lines, causes an in-position check. Because of the look ahead processing, the line with the first G9in successive order will use the in-position check. See also G4 and M95 forother forms of in-position check.

April 2003Section 3: G Codes51FadalUser ManualEXAMPLE:X1.0 G9 (Because of the look ahead, the first G9 will be an in-position check).X2.0 G9 (In-position check).X3.0 G9 (In-position check

G5 Non Modal Rapid The G5 code is used for non modal rapid moves. It exhibits the same motion asG0, however, this code will only affect the line in which it exists. EXAMPLE:X2.5 G1 F20.G5 Z.1 (Rapid movement of this line only).X3.0 Y-2.5 (The G1 is still in effect from above).

 

[Delw]

M94 Feed Forward FunctionThe M94 code is used for linear moves only, to increase accuracy during highspeed surfacing where radical changes in direction occur. These moves aregenerally at a feed rate of 50 ipm or higher. CNC programs for 3D surfaces usemany small linear moves (G1) to form surfaces and the G8 code is used toeliminate hesitation between each move. In most cases this is desirable,except where radical changes in direction occur.Figure 2-3 Feed Forward FunctionThe Feed Forward function affects the way the control accomplishes theacceleration and deceleration at the beginning and end of each move. When amove falls into the range assigned by the M94 parameters, the control willmonitor axis servo feedback to determine how to move, instead of usingreprocessed moves as it normally would.SPECIAL FEATURE9P WORDXXOF MOTIONDIRECTIONNOT APPLIEDDECELERATIONAPPLIEDDECELERATIONANGLETHE Q WORD LENGTHMOVE IS LESS THANWHEN THE PREVIOUSTHIS ANGLE IS USED Q WORD LENGTHLESS THAN

40Section 2: M FunctionsApril 2003FadalUser ManualThe M94 and its parameters must be on a line with NO other codes. It is modaland is canceled by an M95. It only operates with the -3 processors or higher,and is not operational in the G91.1 mode. Deceleration occurs when the angle between moves is smaller than the P wordand the move length is greater than or equal to the Q word. The Q word is not arequired parameter, and is used to filter out extremely small moves.M94 P91 Q.003 (This sets the decel/accel for any move that is both .003 or longer and smaller than 91 degrees from the last move).P WordThe P word sets the angular tolerance for the feed forward mode, and must beless than 180 degrees. When the angle between the current direction and thenext programmed direction is less than the P word, the machine initiates a highspeed deceleration to increase the accuracy of the directional change.Acceleration then begins regardless of the length of the following moves. Theacceleration may occur over an unlimited number of program blocks. Fullacceleration is accomplished over a distance of two hundred thousandthswhen no further deceleration is required.Q WordThe Q word is used to set the length tolerance for the feed forward mode. Whenthe length of the next programmed move is equal to or longer than the Q word,the control checks the angle between the current move and the next move. Ifthis angle is less than the P word value, deceleration occurs.Note: M94 and M94.1 can both be in effect at the same time.M94.1 Feed Forward by Feed Rate ModificationThe M94.1 code is another type of feed forward mode used for high speedsurfacing. The feed rate will be modified if the angle of the next move falls inthe range established by the parameters of the M94.1 code line.No other codes can be in the same line as the M94.1 and its parameters. Thefeed rate must be specified before the M94.1 line. No other F Word may bespecified after M94.1 until an M95.1 is used. G0 moves can be used afterM94.1 but will not be modified by the M94.1 coding. The M94.1 is modal andis canceled with an M95.1 code. It is available on -3 or higher controls. This isnot compatible with the G91.1 code.M94.1 P170 Q10. R0+50. R1+1. R2+15. TIME SAVER

April 2003Section 2: M Functions41FadalUser ManualEXAMPLE:The second move is 135 degrees from the first move, therefore the feed will bemodified because the move is less than 170 degrees (set with the P word).Because the second move is less than one inch (set by the R1+1 word), thefeed will be modified. The angular difference between the P word angle and thesecond move is 35 degrees. Every 15 degrees of angular difference (R2+15.),the feed will be modified by 10 percent (Q10). In this case the feed will bemodified by 20 percent. In order for a move to be modified, it has to be lessthan the P value and less than the R1 value.P WordThe P word represents an angle. If the angle between the current move and thenext move is less than the P word angle, the feed rate will be modified.Q WordThe Q word represents a percentage. This will be the amount that the feed ratewill change each time it is modified (see R2 below for frequency of themodification).R0+#Figure 2-4 R0+#The R0+# represents a percentage. This states that the modified feed rateshould reduce no more than this percentage of the programmed feed rate.R1+#The R1+# represents a length. This states that if the next move is longer thanthis amount, then use the programmed feed rate for that move.R2+#The R2+# represents angular degrees. With the Q word modificationpercentage, this will be used to determine how the feed will be modified. Thiswill modify the feed rate (by the percentage assigned to the “Q” word) everyR2+# degrees for the current difference in angular moves by the percentageassigned to the “Q” word.EXAMPLE:N15 F100. G1SPECIAL FEATURE9THIS RANGEMOVE IS WITHINUSE M94.1 IF DIFFERENCEANGULAR

42Section 2: M FunctionsApril 2003FadalUser ManualN16 M94.1 P170 Q10. R0+50. R1+1. R2+15.The modified feed rate would be determined by this formula:Fmodified = Fprogrammed - (Fprogrammed • Q word • Angular Difference / R2+#)With an angular difference of 60 degrees and a programmed feed rate of 100. ipm, the modified feed would be 60 ipm:Fmodified = 100. - (100. * .1 * 60. / 15.) = 60.Note: M94.1 and M94 can both be in effect at the same time.Note: The feed rate to be modified must be specified before the M94.1. Noother F Word may be specified after M94.1 until an M95.1 is used. A newfeed rate may be specified and then the M94.1 can be used again.

M94.2 Advanced Feed Forward The advanced feed forward option is designed to satisfy the needs of highspeed machining. Normally the gain, acceleration rate, deceleration rate, anddetail factor on a machine tool is established to satisfy a large range ofcustomer needs. Until now this did not directly target the specific needs of highspeed contouring on surfaces. AFF allows the user to tune the machine tospecific needs.Production rate is important! AFF allows the machine to cut loose and fast forroughing cuts, tighter for semi-finish cuts, and very close tracking for finishcuts.One method for controlling surface integrity is feed rate. Other controls will usewhat is termed “look ahead” to analyze angular change in a series of moves.The more dramatic a change, the lower the feed rate. This results in lower cycletimes. AFF differs in that the feed rate is constant resulting in faster cycle times. AFF allows five factors to be altered:•Gain•Deceleration•Acceleration•Detail•Feed RateOPTIONAL FEATURE9

April 2003Section 2: M Functions43FadalUser ManualThese factors can be altered on-the-fly, can be hard coded in the program, orthe parameters can be used from and stored in a parameter page.•Use the DFF command to access the parameter page.•Use the background edit menu to alter the parameters and changethem on-the-fly.•Use parametric variables to hard code the parameters in the program.R1Deceleration: The time to decelerate the axes from programmed feed rate toa full stop measured in milliseconds. Deceleration is important to slow the tooldown for smooth transitions into or around corners. The deceleration willimprove the ability of higher feed rates to be used. At higher feed rates, a largerdeceleration may be necessary to provide a smoother transition into thecorners and to meet the specified detail. There is a point when the decelerationwill not improve the quality of the part but will adversely affect the total parttime. Pick a deceleration value that gives good part times while meeting thedesired tolerances of the part. Values of 20 to 80 are appropriate for most feedrates. The deceleration ranges from 5 to 250 milliseconds.R2To pick up values from the DFF table, set the value of R2 to the correspondingtool number in the table. The parameters will then be used from the table.P WordAcceleration: The time to accelerate the axes from a full stop to theprogrammed feed rate measured in milliseconds. The tool is accelerated out ofcorners or part details to the programmed feed rate. This is the approximatetotal time for the acceleration curve to bring the tool up to full speed. Values of10 to 40 are appropriate for most feed rates. The acceleration ranges from 5 to250 milliseconds.Q WordDetail: The minimum detail acceptable is measured in inches. The detailparameter will hold the X, Y, and Z axes to a specified detail amount. This detailwill dynamically change for each axis depending on the contour, but will alwaysmeet the programmed detail value. The ability of the axes to meet their detail isdirectly affected by the other AFF parameters. A larger gain will help the axis be“driven” to meet the detail specified. The deceleration will help the axes tosoftly move from the programmed feed rate down to zero speed and to thedetail desired. The acceleration will not directly help the detail but will helpwhen using faster feed rates. It will improve the transition from zero speed tothe programmed feed rate. The detail value ranges from .0002'' to .0250''. Theappropriate value depends on the part and tool. If it is a roughing tool, a largerdetail should be used.

 

[Delw]

M95 Feed Forward CancelThis code is used to cancel the M94 mode. It is non modal and must be theonly code on the line.This code can also be used as a non modal form of the G9 code. If the programis in the G8 mode, an M95 on a line by itself will affect the next line in theprogram so that it will decelerate and accelerate. After the move is complete,the G8 mode will continue.EXAMPLE:N15 F100. G1N16 M94.1 P170 Q10. R0+50. R1+1. R2+15....N10350 X.001Y-.04N10351 M95 (Cancel Feed Forward).M95.1 Feed Forward by Feed Rate Modification CancelThis code is used to cancel the M94.1 mode. It is non modal and must be theonly code on the line.M95.2 AFF CancelThis code is used to cancel the optional Advanced Feed Forward mode .

 

[Vancbiker]

I believe -4 and 5 are pretty much the same as far as options and codes, Vanbiker might know..............

Sorry no. I escaped from working on Fadals in 1992 and never looked back.

 

[angelw]

I dont think the G05.1 is used that way on a fadal, according to the fadal book its used for a rapid.?

Hi Delw,
Sorry, I had stumbled into this thread not realizing it was Fadal specific; my Post is how it works with a Fanuc control.

Regards,

Bill

 

[Delw]

Hi Delw,
Sorry, I had stumbled into this thread not realizing it was Fadal specific; my Post is how it works with a Fanuc control.

Regards,

Bill

Bill dont be sorry. I had forgot you were on the website and was thinking about pm'ing you about it on the other one.
kinda hoping you can explain a few g and m codes' (listed above). (not the g08 g09 but the other ones)

Reason Frankly I never used them except once from a customers program and didnt understand them and it might be a benifit to use them.
Its always good to get information never too old to learn.