[stevo1]

Psycho, Bill, Kiwi,
Well guys I have to be honest I really didn’t think that I would open up this size can of worms when I started this thread. I really expected 1 or 2 posts with a few lines of code saying “here ya go Stevo”. I suppose if it is going to be few and far between starting my own threads then this is defiantly not doing it half ast. Go big or go home I believe is the popular expression.

The offer is still open for about 700 lines (5 miles) of point to point code if that will help you get some time with the Kids.

Thank you for the offer and I will let you know when I have conceded. This may cause a problem because I think I would have to dripfeed that many lines of code to my control and believe me when I say that could be another 5 page thread trying to set that up. Macros is my gig……short sweet and to the point. For the most part I told the boss I am taking off….however my mind already knows I will be working on this on Sunday anyway

This is going to be for a production job. Right now I have about 40 of these pc ready to run and more to come. I didn’t want to go back and read the 50 or 60 some odd posts in this thread but if I stated it was a 1 off job I apologize for the misinformation.

LOL... Well, there's 3 to choose from for either setting... MAN!

That is what I have been trying to wrap my head around. Its funny you asy it because I have been messing with these along with plane selection to see if anything works. We all know we can pick on the Fanuc manual interpretations all day long. Plane selection I can understand. Interpolation I can wrap my head around when I need to. Plane selection on a 5axis gets foggy. Now we want to throw axis swapping in polar coordinates on top of all 3 along with this being driven by specific parameter settings to do so. “MAN” is an understatement.

From other comments Steve’s made, I believe he operates along the same lines. With Polar interpolation under his belt, he will be able to write programs for applications such as the focus one with no more than a calculator and an understanding of trig; and I'm sure he has that.

You could not be more correct. My first task as a greenie given to me many years ago by my predecessors who had degrees on MT programming and doctorates in mathematics were how to calculate a radius onto an angle. Acad, a calculator and my macro experience is what has brought me to the level that I am at. You would not think that is true with the ignorance that I have shown in this thread but none the less we are here.

From the beginning of this thread I have been going from my gut that this was a parameter setting issue so I am really hoping that it is. I can’t believe that with all the machining/programming experience of you guys posting here that it can stump everyone for this long(group)

Speaking of a long thread………let’s keep this going and maybe we can outpost Psycho’s thread on MT porn in the PM forum (still following it).
Psycho……I am actually really surprised that Fritz has not chimed in once or twice hey!!

You guys really have no idea how much I appreciate the help and time you have committed:cheers:
Steve

[Kiwi]

...Thank you for the offer and I will let you know when I have conceded. This may cause a problem because I think I would have to dripfeed that many lines of code to my control and believe me when I say that could be another 5 page thread trying to set that up....

If you hit the brick wall and need use the point code, the single lug code can have a variable added to the B angle so the program would be about 70 line all up.

[psychomill]

LOL..... I imagine with part due dates and what not, that brick wall just may come up pretty quick! Longhand will get the job done, no doubt.
The absolute code for Polar works as I did run it in my machines. For Steve, I think it's a matter of getting 1032 and 1033 set up right... I'll look at that more later or post a tweaked loop program....

The I code posted was for one lug only. I can supply code for all the lugs.
My suggested method is for segment moves (using B axis and Z travel) around the lugs and the B axis to rotate between the lugs.

If you hit the brick wall and need use the point code, the single lug code can have a variable added to the B angle so the program would be about 70 line all up.

Hell Kiwi... Don't hold out! Throw it up here! The input is well worth considering I'm sure.

Speaking of a long thread………let’s keep this going and maybe we can outpost Psycho’s thread on MT porn in the PM forum (still following it).
Psycho……I am actually really surprised that Fritz has not chimed in once or twice hey!!

ROFLMAO!!! Isn't that a riot!?!? That thread has over 40,000 hits.... it's like damn YouTube vid or something. I am surprised it still pulls many posts to this day considering I started that one back in August of '08! 3 years and still running.....
Of course, what am I talking about... I'm still dickin' around with those things 3 years later (chair) ... and more fun to come still!

I honestly believe though, we're damn close and I think it's locked into your parameters. I think Bill will be of great help here since I can't find the right machine parameters for you from my old FANUC machines I used to have. Again, I'll mow over the book and see if a light bulb comes on...

[Kiwi]

....Throw it up here! The input is well worth considering I'm sure...

I don't know Fanuc format and I'm sure it will need to be corrected.
This code is in steps of 0.5 deg around each lug, and continuous between lugs.

#100 = 0
G01 X0 Z16.983 B0
N01 IF [#100 GE 360] GOTO 2
G01 Z16.983 B9.2025+ #100
G01 Z17.1826 B9.7025+ #100
G01 Z17.288 B10.2025+ #100
G01 Z17.3448 B10.7025+ #100
G01 Z17.3649 B11.2025+ #100
G01 Z17.365 B11.25+ #100
G01 Z17.3649 B11.2975+ #100
G01 Z17.3448 B11.7975+ #100
G01 Z17.288 B12.2975+ #100
G01 Z17.1826 B12.7975+ #100
G01 Z16.983 B13.2975+ #100
#100 = #100 + 22.5
GOTO 1
N02 G01 Z16.983 B360

[angelw]

Hi Steve,
I can supply you with script that you will be able to write into a Fanuc User Macro routine.

The script calculates an incremental B and Z move that equates to a constant angular move on the 0.415 plus .25 cutter rad. This is different to a constant angular move of just the B axis and will result in a uniform finish around the lug.

PM me your email if this is of interest and I’ll send it.

Attached is a screen dump of the resulting back plot.





Regards,

Bill

[Kiwi]

Good thinking, here is the formula that I used in my VB Program:
Opp = LugCentreRad * Sin(Angle)
Z1 = Sqr(LugCentreRad ^ 2 - Opp ^ 2)
Z2 = Sqr((LugRadius + CutterRadius) ^ 2 - Opp ^ 2)
Z = Z1 + Z2
B = Angle

[Kiwi]

OK, I've never written a macro before and don't use Fanuc GCode but here is my contribution. Some may find some logic in it.
This code steps around each lug while B rotates and continuous between lugs. This is all absolute.

#100 = 0
#110 = 16.7;Lug Centre Radius
#111= 0.415;Lug Radius
#112= 0.25 ;Cutter Radius
#113= 9.2025;Lug Start Angle
#114= 11.25; 1st Lug Angle
#116 = .01 ;Deg Increment
#117 = 16.983;OD Path Dia.
#118 = 22.5 ;Lug Spacing Angle

G01 Z#117 B0

N01 IF [#100 GE 360] GOTO 5

#115= #114 - #113

N02 If [#115 GE 0]
G01 Z(Sqr(#110 ^ 2 - (#110 * Sin(#115)) ^ 2))+(Sqr((#111 + #112) ^ 2 - (#110 * Sin(#115)) ^ 2)) B#114 - #115 + #100
#115 = #115 - #116
GOTO 2

#115 = 0

N03 If [#115 LE [#114 - #113]]
G01 Z(Sqr(#110 ^ 2 - (#110 * Sin(#115)) ^ 2))+(Sqr((#111 + #112) ^ 2 - (#110 * Sin(#115)) ^ 2)) B#114 + #115 + #100
#115 = #115 + #116
GOTO 3

G01 Z#117 B#114+(#114-#113)+#100

#100 = #100 + #118
GOTO 1

N05 G01 Z#117 B360

[Kiwi]

Modified my program to step around lugs by degree increments.

#100 = 0
#110 = 16.7 'Lug Centre Radius
#111 = 0.415 'Lug Radius
#112 = 0.25 'Cutter Radius
#113 = 9.2025 'Lug Start Angle
#114 = 11.25 ' 1st Lug Angle
#116 = 5 'Deg Increment Around Lug
#117 = 16.983 'OD Path Dia.
#118 = 22.5 'Lug Spacing Angle

G01 Z#117 B0

10 If [#100 GE 360] GoTo 50

#120 = (Atn((Sqr((#112 + #111) ^ 2 - (#110 * Sin(#114 - #113)) ^ 2)) / (#110 * Sin(#114 - #113))))
#121 = #120

20 If [#120 LE 90] Then
#115 = Atn(((#112 + #111) * Cos(#120)) / (Sqr(#110 ^ 2 - ((#112 + #111) * Cos(#120)) ^ 2)))
G01 Z(Sqr(#110 ^ 2 - (#110 * Sin(#115)) ^ 2)) + (Sqr((#111 + #112) ^ 2 - (#110 * Sin(#115)) ^ 2)) B#114 - #115 + #100
#120 = #120 + #116
GoTo 20

#120 = 90

30 If [#120 GE #121] Then
#115 = Atn(((#112 + #111) * Cos(#120)) / (Sqr(#110 ^ 2 - ((#112 + #111) * Cos(#120)) ^ 2)))
G01 Z(Sqr(#110 ^ 2 - (#110 * Sin(#115)) ^ 2)) + (Sqr((#111 + #112) ^ 2 - (#110 * Sin(#115)) ^ 2)) B#114 + #115 + #100
#120 = #120 - #116
GoTo 30

40 G01 Z#117 B#114 + #114 - #113 + #100

#100 = #100 + #118
GoTo 10

50 G01 Z#117 B360

[Kiwi]

Steve. Did you get your mill to run the Polar Interpolation macro? Just interested in your progress.

[Kiwi]

.....I can supply you with script that you will be able to write into a Fanuc User Macro routine....

Bill..Any chance of posting your script here so we all can learn from your work?

[angelw]

Bill..Any chance of posting your script here so we all can learn from your work?

Hi Kiwi,

My approach is slightly different, but the math on the most part is similar and is in expanded form for the purpose of explanation. Accordingly, the program could be made much more compact my combining some of the math.

This program is based on calculating the B axis move relating to a constant angle index about the center of the 0.415 radius, not a constant index of the B axis itself. To do the latter would result in varying facets around the circumference of the 0.415 radius.

There is a variable for the tool radius (#15). I have just hard coded a value in this example, but you could grab this from the System variable associated with the Tool Radius Offset for the tool being used. Accordingly, if you do this, the size of the part can be controlled with Tool Radius Offset, or take a rough and finish cut using the same code. This feature requires, however, that start angles of the lug and the Z start coordinate be calculated in the program

I have checked the Macro code reasonably well, but I haven’t had a chance to check it on a machine to test for syntax errors due to transcribing. The CNC code generated by my script works correctly and the attached back plot picture uses B axis angle moves; it’s not a XY plot.



If the angular increments are made too small, Feed Rate may not be able to be achieved. This is due to Acceleration/Deceleration at the start and end of each block. There simply won’t be enough distance in the block for the machine to achieve the requested Feed Rate.

The program as is will result in conventional milling, which I don't favor. I did the code before I realized the resulting direction. The code in Red will calculate the start point on the other side of the lug for Climb Milling and some sign changes in other areas would be required

Regards,

Bill

‘Initialize some of the variables
‘If the cutter radius size is obtained from the Tool Radius System variable, then the code for that needs to be added here.
#15 = 0.25 'Tool Radius – could be got form Tool Rad System variable
#24 = 0.1 'Incremental angle
#1 = 0 'Large Circle Centre X
#2 = 0 'Large Circle Centre Y
#3 = 16.733 + #15 'Large Circle Radius + TR

#4 = 0 'Small Circle Centre X
#5 = 16.7 'Small Circle Centre Y
#6 = 0.415 + #15 'Small Circle Radius + TR

‘The following code finds the position of the tool at the start of the 1st lug
‘Get start point for to cut 0.415 radius
#7 = #4-#1
#8 = #5-#2
#9 = SQRT[#7*#7 + #8*#8]
#10 = [#9*#9 + #3*#3 - #6*#6] / [#9*2]
#11 = ABS[#3*#3 - #10*#10]
IF[#11 LT 0.00002]TH #11=0

‘1 This code will find the 10 o’clock position of the cutter on the 0.415 radius. Use this if you rotate the B axis counter clockwise
('X1 #12 = #1 + #7*#10/#9+[#8/#9] * SQRT[#11] )
('Y1 #13 = #2 + #8*#10/#9-[#7/#9] * SQRT[#11] )

‘2 This code will find the 2 o’clock position of the cutter on the 0.415 radius. Use this if you rotate the B axis clockwise
#12 = #1 + #7*#10/#9-[#8/#9] * SQRT[#11]
#13 = #2 + #8*#10/#9+[#7/#9] * SQRT[#11]

‘Only use one of 1 or 2 above and delete the other.

'Initial Vertical side of small rad triangle
#16 = #13 - #5

'Initial Horizontal side of small rad triangle
sng665Y #17 = #12 - #4

'Small radius start angle
#18 = ATN[#16 / #17]

''Get start angle of big circle
#19 = ATN[#12 / #13]

'Half of B axis move between lugs
#20 = 11.25

All of the above just primes the rest of the program and only needs to be visited once, or when the tool radius is altered.

‘Go to a clearance position in X,Z and B
G00 G90 X0.500 Z #3 + 0.500 B0.000
Get down to depth here
G01 X0.500 Z #3 F400
G01 X0.000

'Initialize #21 and #22. #22 is used as a multiplier for the move to the next lug. 'Its set to 2 after the move to the first lug is made so that subsequent moves will be based on 22.5 deg
#21 = 0
#22 = 1

Following are the calculations for the moves, both major between lugs, and minor around lug. I didn’t use a WHILE DO END approach as the condition that controls that can be a bit variable depending on the angle increment used. The code between N100 and N200 is to get the tool to the start point of each lug. The code between N200 and GOTO200 is for the Z B moves to generate the lug profile

N100
'Initialize #23 at the start of each new lug for use in calcs
#23 = #18

‘Get the center line angle of the next lug
'#21 = #21 + #20 * #22

'Check for having gone full circle
IF [#21 GT [360 - #20]] GOTO 300

‘Get the B move to start of lig
#29 = #21 - #19

‘Move the B axis
G01 B#29

N200
'Add the incremental angle move to current angle
'#23 = #23 + #24

'To ensure the correct finish point – needed because the incremental angular move may not go evenly into the total angle from start to finish evenly.
IF [#23 GT [180 - #18]] THEN #23 = 180 - #18

'Get the length of vertical side of 0.415 + tool rad triangle
#16 = SIN[#23] * #6

'Get the length of horizontal side of 0.415 + tool rad triangle
#17 = SQRT[#6 * #6 - #16 * #16]

'Get the next Z move
#25 = #5 + #16
#26 = SQRT[#25 * #25 + #17 * #17]

'Get the Angle move
#27 = ATAN[#17 / #25]

‘Change the sign as the cals flip over 12 o’clock
IF[#23 GT 90] THEN #27 = -[#27]

‘The B move is
'#29 = #21 - #27

‘Move in Z and B
G01 Z#26 B#29

'If finish angle not reached - do again
IF[#23 LT [180 - #18] GOTO200

'Set #22 = 2 so that subsequent moves to next lug will be 22.5 deg
#22 = 2

‘The lug end angle was reached – go back to the major B move code
GOTO100

‘GOTO sequence number if the last lug has been machined
N300

'Full circle - next B move is to start point
'#29 = 360

‘Blend off of part and go home vertically – I think the Y axis in your machine
G01 B#29
G01 X-0.500
G01 X-0.500 Z #3 + 0.500 B0.000
Go home vertically

[Kiwi]

.....'Initial Horizontal side of small rad triangle
sng665Y #17 = #12 - #4.....

Bill, looked through your code and this line confuses me. Can you explain the 'sng665Y' please.

[stevo1]

Hey guys,
I apologize for the late responses on this. I have had a very busy week professional and personal so I have not had a lot of time if any to put towards this at the moment. The machine has also been down all of last week due to a blown resistor on the drive board. Fixed that and now have another problem with the drive but at least I can prove out code now, I just can’t run the spindle.

I will be trying a few things today and tomorrow and will report back.

Steve

[stevo1]

Alright guys. I have a good update for you.

I spent this weekend looking thru the parameter and operator manual and comparing these to some machines I have had over the years and put some common sense and logic into this. It was actually quite like a slap in the face when I saw it (with the help of everyone of course). As already stated it was indeed parameters 1032 and 1033 that needed to be corrected. 1033 was set properly at 5(I think). However 1032 needed to be set to 3 (designated Z) to use the Z axis with the B axis in this application. With it previously being set to 1 is was trying to use X (designated 1) and B giving me very strange results.

I now ran my original program and it looks great for the first 230deg or so.

So now I am down to 1 problem and 1 question.

Problem1
I am still getting the OT512 EXCESS VELOCITY alarm. I only get it once it reaches about 230deg around the part. I have my feeds at 160IPM on the rotary movements and 25IPM around the lugs. This is slower then what I want to run. Parameter 1422 is set to B=72 and Z=500. How can I get around this issue?? Why would it only happen once I am 2/3 around the part? I deactivate with 13.1 at every rotation and only activate 12.1 at the lugs.

Question1
Psycho…..you gave me numbers to run the lug if my original program worked along with polar coordinates.
G3B.6204Z.3709R.665F#5
G3B.6068Z-.3928R.665
Am I missing something as these numbers are different then my original numbers?
G3B.6068Z.382R.665F#5
G3B.6068Z-.382R.665
Does using polar have an effect on this? LOL IOW what numbers are right?

Bill,
I am going to also run the macro that you gave me. I would like to see it operate.

Steve

[stevo1]

FYI…….I even ran it at 60ipm around the entire part well under any setting in the 1422 parameter and I get the same alarm at about 230deg.

Steve

[Kiwi]

G3B.6204Z.3709R.665F#5
G3B.6068Z-.3928R.665
Am I missing something as these numbers are different then my original numbers?
G3B.6068Z.382R.665F#5
G3B.6068Z-.382R.665

These pics should help.

[Kiwi]

Bill..Copied and pasted your program into VB and altered to run in VB.
This is the code produced for the first lug with increments of 20 deg.

G00 G90 X0.500 Z17.483 B0.000
G01 X0.500 Z16.983 F400
G01 X0.000
G01 B11.2857349779019
G01 Z17.1500502155777 B11.2210705663942
G01 Z17.3347912185892 B11.2383536908619
G01 Z16.7872723922466 B11.2106242467224
G01 Z16.1305234449828 B11.2290771005863
G01 Z16.1626677510754 B11.2738478035288
G01 Z16.8433301165424 B11.2887210546858
G01 Z17.3492253976892 B11.2584589635203
G01 Z17.1069450203916 B11.2811182693157
G01 Z16.3870782415292 B11.2854719789317
G01 Z16.0516744495906 B11.2590384720939
G01 B33.7857349779019

Doesn't look correct. Not sure what's wrong.

This is what I get with my version when arcing around first lug.
G01 Z16.983 B0
G01 Z16.982978 B9.2025
G01 Z17.084164 B9.408659
G01 Z17.173657 B9.670755
G01 Z17.248532 B9.980809
G01 Z17.30631 B10.329392
G01 Z17.345062 B10.705912
G01 Z17.363483 B11.098941
G01 Z17.365 B11.25
G01 Z17.354498 B11.646188
G01 Z17.323347 B12.030356
G01 Z17.272596 B12.390845
G01 Z17.203948 B12.716705
G01 Z17.119682 B12.998031
G01 Z17.022567 B13.226262
G01 Z16.983 B13.2975
G01 Z16.982978 B31.7025

[psychomill]

Stevo,

The numbers I gave are going to be a bit different than what you originally started with. The reason for this is as Kiwi's pictures illustrate, the effect comes from the fact that the table rotary motion is swapping the linear axis motion. Also, since I think that's from the incremental posting, this is a bit of uncharted territory even for me. I'm always in absolute mode doing this.

As for the alarm.... something in the machine's acc/dec settings is not a happy camper (see attached pic from the FANUC 15m Maintenance Manual). The problem can be from a number of things though and not necessarily your feedrates. Rotary motion is controlled by a variety of parameters and conditions. The "straight up" rotary milling that you're used to doesn't always use the same parameters when not in Polar mode. Also, since these lugs are relatively "tight" in comparison of the OD, the physical positions and distance from CL creates different circumstancesj for the machine to comp for. I'd say that doing this lug on a 10" diameter with the same machine probably won't give you this alarm.

I'm not sure if inverse feed is valid since polar is axis swapping with the rotary so that may be crazy anyway....

Going long hand might be the thing to do for now to knock the parts out. Might need a little factory help to set up the parameters right and even a little tweaking with the servo parameters? I'll dig around some more....

[angelw]

Bill..Copied and pasted your program into VB and altered to run in VB.
This is the code produced for the first lug with increments of 20 deg.

G00 G90 X0.500 Z17.483 B0.000
G01 X0.500 Z16.983 F400
G01 X0.000
G01 B11.2857349779019
G01 Z17.1500502155777 B11.2210705663942
G01 Z17.3347912185892 B11.2383536908619
G01 Z16.7872723922466 B11.2106242467224
G01 Z16.1305234449828 B11.2290771005863
G01 Z16.1626677510754 B11.2738478035288
G01 Z16.8433301165424 B11.2887210546858
G01 Z17.3492253976892 B11.2584589635203
G01 Z17.1069450203916 B11.2811182693157
G01 Z16.3870782415292 B11.2854719789317
G01 Z16.0516744495906 B11.2590384720939
G01 B33.7857349779019

Doesn't look correct. Not sure what's wrong.

This is what I get with my version when arcing around first lug.
G01 Z16.983 B0
G01 Z16.982978 B9.2025
G01 Z17.084164 B9.408659
G01 Z17.173657 B9.670755
G01 Z17.248532 B9.980809
G01 Z17.30631 B10.329392
G01 Z17.345062 B10.705912
G01 Z17.363483 B11.098941
G01 Z17.365 B11.25
G01 Z17.354498 B11.646188
G01 Z17.323347 B12.030356
G01 Z17.272596 B12.390845
G01 Z17.203948 B12.716705
G01 Z17.119682 B12.998031
G01 Z17.022567 B13.226262
G01 Z16.983 B13.2975
G01 Z16.982978 B31.7025

Kiwi,
Below is the code generated by my VB program using 20 deg increments you state you used in your example. Given that there are 131.683 deg between the start and finish on any one lug, there are approx 6.5 bites of 20 deg in that total angular move. Accordingly, I'm unsure how you are able to get 14 x 20 deg moves in there. You will note in my example code below that I have 7 moves after first angle, this is because I force the tool to always finish tangent to the lug radius and the 16.733 radius before moving to the start of the next lug; hence the part move in the approx 6.5 becomes the 7th move to the end angle.

A better approach would be to round the angular move to the closest value to the specified angle, that will go wholly into the total angular move. Not doing so would not be noticeable with moves that will give a good finish around the lug.

Regards,

Bill

G00 X-0.500 Z21.9830 B0.0000
G01 X-0.500 Z16.9830
G01 X0.0000
G01 B9.2025
G01 Z17.1699 B9.6578
G01 Z17.3009 B10.2900
G01 Z17.3617 B11.0266
G01 Z17.3456 B11.7873
G01 Z17.2543 B12.4900
G01 Z17.0979 B13.0568
G01 Z16.9830 B13.2975

[stevo1]

Found some more stuff on the 1422 parameter (see attached). I think that I have to up the 1422 parameter to 360. I will give it a go today if I have time and let you know what happens. If anyone has any other suggestions for parameters to look at please feel free to point them out.

Thanks,
Steve