G3 using a rotary axis??

[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....

[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

[psychomill]

Stevo.... the picture is perfect and clears up much... The mechanical configuration is similar to my Mazak eMachines.

Next question is what is the normal axis directions on this machine? On your machine, "up and down" is Y-axis, the table (or the part) is sitting on the B rotary. From I can tell, the machine is a "5-axis HMC" in relation to axis directions correct? So this would make your spindle rotary the A-axis?


From your macro, looks like you program normal to the standard machine axis directions right? (I use 3D Coordinate Rotation a lot so my axes roll around depending on my head angle).



PS: My machine is 'normally' vertical so the axes are like a VMC. My 2 rotary points are the table carries C and the spindle carries B. Up and down with my spindle is Z axis.

[stevo1]

Yes that is correct. The spindle axis rotation is ”A”. Everything else is as you stated above.

When I rotate my spindle to A-90 (vertical) I use the G18 work plane and the Y-axis is up and down from the table as the Z direction would be on a standard VMC. The Z-axis acts as the Y-axis on a standard VMC.

I should have posted my code earlier as it may have made things a bit more clear. It’s really straight forward and that is probably why it drove me nuts at first that it would not work. Now realizing that it needed polar coordinates it makes me fell less like a doofis. I don’t have slightest idea of what is all wrapped into using this G12.1 as this is a first for me.

As you can see by the code I have B0 as the CL directly between 2 scallops. I can rotate to the first scallop right at the .250 radius but I just can’t seem to get around the scallop properly. Once I can then the macro will just repeat that same section of code.

It always looks easier on paper hey!!

Thanks again,
Steve

[psychomill]

I gotta run now because I've got a major fire to put out.. BUT, if you're up to it, you can give this a whirl.....

in Polar programming your rotary axis is simply taking the place of a linear axis. This is true with the code as well. If I remember right, I used to post code then edit the output by swapping my own rotary/linear axes with an editor (this was some years ago before I got posts that supported Polar programming for machines).

In my shriveling mind, this is how I made this work:

Program your profile as "normal" without rotary just as if you had the travel on a big machine to walk the tool around the whole part. Post the code. Now it's just a matter of swapping the stationary linear axis with the rotary axis (keep all signed directions [+ & -] the same).

So, in your case, your "normal" output would be a profile cut with ZX positions. Now on an editor, just simply swap all your "X" letters with the letter "B". Everything else stays the same. Cut this into your program and use G12.1 and it should cut your arcs.

Here's a short snip of what I'm talking about. This is using my machine (I think you'll get the idea for yours):

Normal XY profile output
X16.983Y0.
G12.1
G1X16.983Y0.
G2X16.7277Y-2.9338I-16.983J0.
X16.5771Y-3.6909I-.3162J-.3306
X14.3316Y-9.1119I-16.5771J3.6909
.
.
.
G13.1

For my machine, I swap "Y" with "C"
X16.983C0.
G12.1
G1X16.983C0.
G2X16.7277C-2.9338I-16.983J0.
X16.5771C-3.6909I-.3162J-.3306
X14.3316C-9.1119I-16.5771J3.6909
.
.
.
G13.1


As stated for your machine, I think if you just spit out ZX profile program, then just swap the X output with B, this will work....


Sorry, may or may not be the right way but my brain is at Mach 3 right now...
Gotta run.... My "fire" is going out of control now....

[Kiwi]

...Steve, You can use the code I posted if change your set to run in this direction.....

WARNING: Steve, I would check the code as the lug profile and radius position are not as your drawing.