[stevo1]

Hey guys I am looking for some help. I had about 10min today to try some code on a new part between putting out fires all day. I would love to get back on the machines and get this going on my own but I don’t get much time on the machines these days.

Attached is a pic of a new part that I need to machine in my 5axis. I am doing this vertically on a 15 series Fanuc control with a rotary axis. The OD of the part is a solid pc that I am milling scallops out of with a 1/2dia endmill. There are 16 scallops spaced around the OD of the part.

I am just bringing my Y-axis (Z on my machine) to the 33.466 dia at CL and rotating the B-axis to the first scallop cc from CL. Now once I start to spin around the scallop via G3B()Z()R() it wants to move the X-axis. I want to keep my cutter/table at X0 and only rotate B-axis.

So this may be a newbie question but with my time constraints I need to know if I can spin around the scallop via G3 without moving the X-axis??
As always thank you for the input.

Stevo

[stevo1]

UPDATE!!

Alright guys I had about 20min minutes today to get on the machine when the boss got out of my hair and went to a meeting.

My statement earlier about the X-axis moving is actually happening but when I ran the code it started and ended where it needed to be. The X-axis movement in-between I ass u me is a must to complete the arc??

Here is the code that I ran. Can anyone confirm that this is correct per the sketch?

G0B0Z16.938Y.1
G1Y-.1
G91B9.2025
G3B2.0475Z.382R.3325
G3B2.0475Z-.382R.3325

This code starts at CL and dia of part at B0. Table rotates 9.2025 to first scallop which tucks the .5” endmill nice right in the corner .250” radius. G3 runs up to the top of the scallop then back down to the .250” radius.


Gotta run....kids are calling!! I will check back tonight from home.
Thanks,
Steve

[Kiwi]

...Z16.938...

Should this not be Z16.983? (33.466/2)+0.25

I don't have a 4th axis so unable to confirm your if code will do what you require and if it is possible to have the rotating axis interpolate using G2/3.

[stevo1]

Yes you are correct that it should be Z16.983. That was my typo. I actually have all of this coded through variables in the macro that I wrote and I just put hard numbers in this post to make it easier.

My suspicion was confirmed lastnight from over at the PM forum that this may have to do with using the polar coordinate option in the control. I had this once before on a vertical lathe with live tooling. I did not work on the project but was told that was the issue.

I have been pulled off the project for now but will report anything that I come up with. Please if anyone has any other suggestions of what could be the issue let me know.

Stevo

[Kiwi]

...Please if anyone has any other suggestions of what could be the issue let me know....

If you can't get the G3 to work here is some code which you may be able to use.

B9.203 Z16.9833
B9.303 Z17.0372
B9.403 Z17.0818
B9.503 Z17.12
B9.603 Z17.1534
B9.703 Z17.1827
B9.803 Z17.2089
B9.903 Z17.2321
B10.003 Z17.2529
B10.103 Z17.2715
B10.203 Z17.2881
B10.303 Z17.3027
B10.403 Z17.3157
B10.503 Z17.3269
B10.603 Z17.3366
B10.703 Z17.3448
B10.803 Z17.3516
B10.903 Z17.357
B11.003 Z17.3609
B11.103 Z17.3636
B11.203 Z17.3649
B11.25 Z17.365
B11.297 Z17.3649
B11.397 Z17.3636
B11.497 Z17.3609
B11.597 Z17.357
B11.697 Z17.3516
B11.797 Z17.3448
B11.897 Z17.3366
B11.997 Z17.3269
B12.097 Z17.3157
B12.197 Z17.3027
B12.297 Z17.2881
B12.397 Z17.2715
B12.497 Z17.2529
B12.597 Z17.2321
B12.697 Z17.2089
B12.797 Z17.1827
B12.897 Z17.1534
B12.997 Z17.12
B13.097 Z17.0818
B13.197 Z17.0372
B13.297 Z16.9833

[psychomill]

Stevo..... what Kiwi posts is another way to do it and you don't need to use polar commands....

Your program just ends up being 17 miles long though....

[Kiwi]

...Your program just ends up being 17 miles long though....

The code posted (with minor changes) could be included in a loop for each lug and the program need not be much longer than what I posted.
Even using the code for each 16 lugs with one line between to rotate B this would be under 700 lines.
If just G2's and G3's was used to go round the circumference, the code would be under 70 lines
Hardly 17 miles long.

[Kiwi]

.... what Kiwi posts is another way to do it and you don't need to use polar commands....

The code I posted needs the polar commands as the part is being rotated on the B axis.
I assume stevo1 is doing it this way because of the disc diameter.

[psychomill]

Ahhhhh Kiwi..... I see you're a person of literal meaning....


The code you posted looks plotted so I'm not sure why you would need polar commands for it? Anyhow, I agree with what you say, 700 lines or so doing it this way.... but that was my only point. Relative to a program using Polar Coordinate Rotation, it's much longer.

Here's code using G12.1 going around the part... this is all 16 lobes and the body diameter in one profile cut all the way around:

G1X16.983C0.
G2X16.7277C-2.9338I-16.983J0.
X16.5771C-3.6909I-.3162J-.3306
X14.3316C-9.1119I-16.5771J3.6909
X13.9028C-9.7537I-.4187J-.1845
X9.7537C-13.9028I-13.9028J9.7537
X9.1119C-14.3316I-.4574J-.0102
X3.6909C-16.5771I-9.1119J14.3316
X2.9338C-16.7277I-.4265J.1656
X-2.9338I-2.9338J16.7277
X-3.6909C-16.5771I-.3306J.3162
X-9.1119C-14.3316I3.6909J16.5771
X-9.7537C-13.9028I-.1845J.4187
X-13.9028C-9.7537I9.7537J13.9028
X-14.3316C-9.1119I-.0102J.4574
X-16.5771C-3.6909I14.3316J9.1119
X-16.7277C-2.9338I.1656J.4265
C2.9338I16.7277J2.9338
X-16.5771C3.6909I.3162J.3306
X-14.3316C9.1119I16.5771J-3.6909
X-13.9028C9.7537I.4187J.1845
X-9.7537C13.9028I13.9028J-9.7537
X-9.1119C14.3316I.4574J.0102
X-3.6909C16.5771I9.1119J-14.3316
X-2.9338C16.7277I.4265J-.1656
X2.9338I2.9338J-16.7277
X3.6909C16.5771I.3306J-.3162
X9.1119C14.3316I-3.6909J-16.5771
X9.7537C13.9028I.1845J-.4187
X13.9028C9.7537I-9.7537J-13.9028
X14.3316C9.1119I.0102J-.4574
X16.5771C3.6909I-14.3316J-9.1119
X16.7277C2.9338I-.1656J-.4265
X16.983C0.I-16.7277J-2.9338


This is is the entire profile and this has shorter line count than the code you posted for one lobe. That was my only point....

"Hardly 17 miles long..." .... OK. You got me. I may have fudged this by a several miles eh? How about 5 or 6 miles? :stickpoke


:cheers:


(note: Stevo, obviously don't use my code unless you plan on rearraging your machine axes! LOL .... )

[Kiwi]

...Here's code using G12.1 going around the part... this is all 16 lobes and the body diameter in one profile cut all the way around:...............
.......This is is the entire profile and this has shorter line count than the code you posted for one lobe. That was my only point....

I agree the code can be written quite simply going around the profile but from what I understand that's not what Steve wants.
Looking at his code he wants to move the cutter along the Z axis while rotating the plate on B axis. He needs the tool to follow the profile and hopes to use G3. He wants confirmation this is possible.
I don't see how your code helps with this setup.
I offered an alternative method. See pics.

[psychomill]

I know what your code is doing... It's plotted and that's fine, nothing wrong with it.

... and you are right Kiwi, ... Steve wants to know if he can use G3 commands using rotary. I'm saying "YES" he can and I posted the code for it. The only difference is that my sample is rotating the C-axis while moving X. Steve is set up to roll B while moving Z.

Again, back to being literal again.... When I stated "going around the part" I didn't mean it as the cutter is going around the part. The code I posted is using the rotary the whole time and it's all in G2.

The only thing different is the axis names. His machine is not set up the same as my 5-axis machine... that is all. He has already confirmed that he has polar command (G12.1) available on his machine.

[Kiwi]

Ok. I don't know Fanuc GCode, and never used a rotary table. Was only trying to help in a way I could see how he could do the job.
I'm sure Steve will be pleased to finally hear confirmation that G3 will do what he wants.

[psychomill]

... Was only trying to help in a way I could see how he could do the job.

... and IMO, you did. As I stated, what you showed is another way to do this.

In the end, you've got a skinned cat. How it got skinned can be any number of ways. I merely focused on how Steve wanted to "skin it" as I'm sure he can plot point code all day long....

It's all good.... :cheers:

[Kiwi]

...what Kiwi posts is another way to do it and you don't need to use polar commands...Your program just ends up being 17 miles long though.....

... I merely focused on how Steve wanted to "skin it"....

On your original post, I don't see any focus on Steve's method?

... I'm sure he can plot point code all day long....

I didn't spend time plotting all these points. I wrote a VB script to generate the code.
I prefer to generate my code this way, rather than using CNC time testing.

[Kiwi]

Can anyone confirm that this is correct per the sketch?
G0B0Z16.938Y.1
G1Y-.1
G91B9.2025
G3B2.0475Z.382R.3325
G3B2.0475Z-.382R.3325

As proven, I'm just a green horn on this, but I'm thinking your R should be R0.665.
Just flame me if I'm wrong, I'm pretty thick skinned.

[stevo1]

Wow. Good info guys. I really appreciate the help on this.

Psycho….I know you asked over at the PM forum about not quite getting your head around how my machine is setup. It is a 5axis machine but I am using it just like a vertical machining center. Picture a vertical with a rotary table instead of a stationary one. The head rotates so I can machine vertically or horizontally. I have the head rotated to point straight down just like a machining center.

Now the rotary axis is commanded by “B”. The up and down or Z on a typical machine is commanded by “Y” on my machine and the standard Yaxis is commanded by “Z”. I also attached a pic of the machine if it will help.

Psycho…….so am I to assume that the above code that you posted will not work in my machine because you are moving in X along with C? Since you say I can use the G3 how is it coded if using the polar coordinates. I tried my code and it gives me a over tolerance of radius. I thought I read in the book that the angular position must be linear number on the cartesian coordinate system so IOW it would be the X distance and not the angular distance?? Does that sound right?

As most know I am a macro guy so I vote for the 1/4mile program length. The shorter the better.

Thanks to everyone again,
Steve

[stevo1]

As proven, I'm just a green horn on this, but I'm thinking your R should be R0.665.
Just flame me if I'm wrong, I'm pretty thick skinned.

I was questioning this myself. The only reason that I thought this would be half the R is because I was spinning the first half then the second half.

Stevo

[psychomill]

Kiwi.... Really!?

Originally Posted by psychomill
... I'm sure he can plot point code all day long....

I didn't spend time plotting all these points.

Kiwi, you're being way too literal and besides, I was remarking Steve's ability here.
and my response to "not needing polar commands" was in response to your program post, not what Steve should do.

That's cool stuff with your script though..... Nice.

Look, we're trying to get Steve to the same place... let's just leave it at that.
(also for note, Steve is posting on 2 different sites which I'm in both of so there may some aspects of the conversations you're not aware of).


Steve,
You can use the code I posted if change your set to run in this direction. This code is rotating C axis while moving in X and the YZ is stationary (side cutting the profile with the endmilll)

I didn't look at your pic so let me get my head around your set up and machine.... be back shortly....

[stevo1]

I didn't look at your pic so let me get my head around your set up and machine.... be back shortly....

Thanks much……FYI I just snapped a pic of the machine this morning and it does not have the part that I want to machine on it. That part is on another pallet that I will bring in when I am ready to go. I just wanted to get a pic so you had an idea of what I am looking at. I ass u me that you only needed a snapshot of the machine?? I can take a few different shots and one of the part but all it entails is a round pc of ally with some toe clamps holding it.

Kiwi…yes I did post over at the PM forum as well after I got no response here at the zone so Psycho has more details. I don’t like double posting but I wanted to keep moving on this and didn’t see any replies in a few days.

Stevo

[stevo1]

I have the program written to do this my only problem is the code to actually machine 1 scallop. This code goes in place of the G3 lines below. I just didn’t want to muddy the waters with macro code but I am thinking it can’t hurt.

Steve


O1111(PROVEOUT)
#1=.5(TOOL DIAMETER)
#2=33.466(DIA TO CUT)
#4=.01(DEPTH OF TOOL)
#5=11.2(RADI FEED RATE)
#6=192(ROTARY FEEDRATE)
#3=100(SPEED)
#10=0(COUNTER)
G0G90G59G18X0Y3.Z[[#2+#1]/2]B0M3S#3
G91X-.5Z.15
G90Y.1
G1Y-#4F50.
G91G2X.5Z-.15R2.F#5
G1B9.2025F#6
N1G12.1

G3B2.0475Z.382R.3325F#5
G3B2.0475Z-.382R.3325

IF[#10GE15]GOTO2
#10=#10+1
G13.1
G1B18.405F#6
GOTO1
N2G1B9.2025F#6
G2X.5Z.15R2.
G0G90Y4.
M30