5-axis and TCP

[Jeremy Herron@DBS Solutions™]

TCP works fine on that style of machine. WSEC gives you more ability, but it really depends on the kinds of parts you run. They can be used together. I would not buy a machine without it, but I am kind of spoiled. So, if money is tight, it really comes down to whether or not you need the ability to adjust for any "skewing" of the part from how it was programmed.

[Reko]

Thank you. I will definitely add it to the list.

 

Also, I added "Tilted Working Plane" and "Cutter Compensation for 5-Axis" and "3-dimensional Manual Feed" to our new Fanuc 31i A5 controller.

 

Can anyone give me a run-down on the uses of these functions and how well they work?

 

I'm new to 5-axis, so sorry about the simple questions.

[Jeremy Herron@DBS Solutions™]

I am a little short on time this morning and I will write more later, but you will to look at these too...

 

AICC, AICC II, High Speed Processing, Extended Block Look Ahead, NANO Smoothing, NANO Smoothing 2, High Speed Smooth TCP, Tool posture control

 

[Reko]

When using TCP on a Fanuc 31i A5 controller, there is a "pivot distance" stored in the controller... where is the pivot distance measured from, and how is it input in the controller?

 

G43.4 H1 Z0

 

...that is the line my post processor outputs...

 

Is H1 referring to tool offset 1? What should I be entering there?

[Jeremy Herron@DBS Solutions™]

Yes H1 is the tool length. It should be the same as it would be regularly. Are you using a clearance plane? If so what is set to?

[Reko]

Clearance plane is 55" (radius) on a 105" diameter part.

 

I'm just at the beginning of trying to figure out how to deal with height offsets on RAH, TCP, AI control, etc.

[Guest]

Ht offsets on a RAH are either pivot point to center of tool (on nutating head type machine) or gage line to center of tool and it'll never change even when you change tools. Which way this is handled depends on your Parameter #19666 value. Zero and you have to comp the whole assembly (pivot point to tip), if there's a vaue there, see what it represents. DIfferent MTB's will use it differently.

 

One thing I've alwaus been tempted to try (never had the time or opportunity though) is to use the Radius/Diameter Geometry offset to Comp the distance of spindle centerline to the tip of the tool. Obvioulsy this won't work for drilling ops, but could possibly work for milling.

 

HTH

[Guest]

Oh, AI-NANO... that's been covered Ad Nauseum for the better part of a decade in here. Do a search for "AI-NANO" or "AICC" and you'll see what I mean.

[Guess_who]

We use strictly DFO on our Jidic HD5 and it works great. We use TCP on our Makino D500, and we had issues getting MasterCam to program it properly. I am only referring to full 5th axis. We ended up programming the Makino with NX. But Mastercam programs the Jidic just fine.

 

When we first got the Makino we have to switch the parameter back to DFO while we reprogrammed the first part in NX.

 

But other that programming, we never had any issues with either one at the machine. I would say it a lot easier to follow the code when using DFO though.

 

Just my 2 cents

[Reko]

Okay, so if I have a RAH and I am working on a round part and drill holes around the perimeter... I set up the centerline and top of the part as X0 Y0 Z0.

 

The X is set at zero in G54 in the center of the part.

The Z is set at zero in G54 at the top of the part at the centerline of the tool.

 

The Y is set at zero in the G54 in the center of the part... but the tool vector is in the Y direction so how exactly do I set that?

Obviously, with a straight head, G43 H01 Z is used... but on a RAH... how is this accomplished?

 

Thanks.

[Guest]

With the RAH, you need to offset the CL of the Spindle to the Tool TIp in your Work Offset... depending on how your post outputs things of course.

[Reko]

Thanks James.

 

Currently, I am using separate work offsets to program the four quadrants using planes.

 

I will contact my post developer to see where to enter the value of the tool tip, to pivot point length.

 

I guess I was hoping for a way to set the pivot length, then program to the center of the part. Possible?

[robk]

One thing I've alwaus been tempted to try (never had the time or opportunity though) is to use the Radius/Diameter Geometry offset to Comp the distance of spindle centerline to the tip of the tool. Obvioulsy this won't work for drilling ops, but could possibly work for milling.

It works great James. You could drill without using canned cycles but obviously you can't tap, but since I prefer to threadmill with RAH this has not been an issue yet. When using G68 I ALWAYS use that route, but on our older machines sometimes it makes sense to use work offsets instead.

 

Reko, after entering the H value (James' decription a few posts above) enter whatever the value is from the C/L of the spindle to the tip of the tool into your Dia/Rad wear comp and call that number with -D- within your program. Use G45 or G46 to activate it (In the other post I showed you a sample where I use a variable instead of actual #, but the results are the same)

 

 

This sample is from a standard 3+2 machine and I use wear comp for tool stickout.

()

(PRE-DRILL .188 HOLES USING RAH)

(18 HOLES)

()

G90 G80 G00 G17 G40 G98 G49

G00 G90 G18 G54 X0.0 Y0.

B0.

C3.7

S1265 M03

G43 Z5.098 H138

G46 Y-3.0195 D138 M08

G83 X0. Z2.533 Y-3.519 R-3.0195 F1.26 Q.05

G80

.

.

.

 

I have not been succesful in using TCP with Right Angle Heads--only G68 (as I posted in another thread) so no true 5 axis, BUT I have been using the RAH for true 5 axis machining using Dynamic Offset and it works great!!!

Daniel posted a thread that I drooled over, but his solution is Sinumerik http://www.emastercam.com/board/index.php?showtopic=71913

[Jrygus]

I just wanted to follow up on this thread. I am still using TCP and it is working great. I had issues with the transition from one rotation to the next, so I had to do a lot of pre-positioning of the tool so that it would not run into the table while it rotated to the next position. But, now I am using Icam's Smartpath software in their simulator and I do not have to worry about that anymore. It calculates the motion between cuts so that you clear your fixtures and material while moving to the next cut. it saves me a lot of time when programming for this machine. It eliminates a lot of strange machine motion between cuts as well. I am still in the Beta testing of it, but it is very impressive.