Using G43.4 for 5-axis machining

[AloneAsAShadow]

My CNC is a Fryer 5x-45 with a Fanuc 18i-MB5 controller. I started using G43.4 (TCP) for 5-axis machining. This seems to cause the machine to jerk really badly. The machine also makes loud bangs when 5-axis machining due to the large change in acceleration. Others have suggested G05, G05.1 and G08 but the controller's manual says those commands are unavailable when using G43.4.

Is there a look-ahead acceleration and deceleration used for G43.4 that could control the jerk?

Any suggestions will be greatly appreciated

[crazy^millman]

Seems the machine needs to be tuned for G43.4 since that is an older control it might not have all the parameters set correctly. The other thing you can do is try inverse time with G93 and see if that helps the issues you are having. Need to be careful with older controls and where you program Zero from. If picking it up like a 3 Axis machine by picking the top of the part that can be creating major issues for the control to adjust feedrates for that position relative to the COR(Center of Rotation). In older machines programming in CAM using COR and inverse time setup correctly corrects this issue. Either way have to be mindful if using G43.4 and not using G68.2 what other problems you might be running into.

[gcode]

you might fid this video useful

 

Making the Cut- Mastercam Toolpath Deep Dives - Industrial Forum - eMastercam.com

[Colin Gilchrist]

There are two ways to go here:

• You can smooth out both the "toolpath tip points", and the "vectors" to reduce the amount of motion and acceleration between each position commanded in the NC Code. Dylan at CNC Software just posted up a video on this very subject. Check the Main Industrial Forum page. This may help you a little.
• You can purchase Smooth TCP & Rotary Axes Compensation (G43.4 P3 & G43.3 L1). These would need to be added by the Machine Tool Builder (through Fanuc). I think the option includes Tool Posture Control, but you'll want to check.
• I'm pretty sure you'll also need to option "Cutting Point Control" as well, to properly use Smooth TCP.
• There is a "High-Speed" option (Nano Smoothing Type 2), which can be used in conjunction with TCP Type 1 (G43.4), however, it won't smooth out the "Jerk" of the Axis Acceleration. This is due to the fact that Nano 2 is really only concerned with converting the "input path" into a NURBS Curve. This only affects the "tool tip trace", and doesn't consider the Tool Axis (Tool Posture), from move-to-move. This is really what High-Speed Smooth TCP is used for. (Smoothing of the "tip motion", or smoothing of the "side cutting".)

[huskermcdoogle]

On 8/9/2021 at 2:44 PM, Colin Gilchrist said:

There are two ways to go here:

• You can smooth out both the "toolpath tip points", and the "vectors" to reduce the amount of motion and acceleration between each position commanded in the NC Code. Dylan at CNC Software just posted up a video on this very subject. Check the Main Industrial Forum page. This may help you a little.
• You can purchase Smooth TCP & Rotary Axes Compensation (G43.4 P3 & G43.3 L1). These would need to be added by the Machine Tool Builder (through Fanuc). I think the option includes Tool Posture Control, but you'll want to check.
• I'm pretty sure you'll also need to option "Cutting Point Control" as well, to properly use Smooth TCP.
• There is a "High-Speed" option (Nano Smoothing Type 2), which can be used in conjunction with TCP Type 1 (G43.4), however, it won't smooth out the "Jerk" of the Axis Acceleration. This is due to the fact that Nano 2 is really only concerned with converting the "input path" into a NURBS Curve. This only affects the "tool tip trace", and doesn't consider the Tool Axis (Tool Posture), from move-to-move. This is really what High-Speed Smooth TCP is used for. (Smoothing of the "tip motion", or smoothing of the "side cutting".)

I don't know if those options are available on the 18i series controls.  If they are, that would be the way to go.

IIRC, and correct me if I am wrong, but Nano Smoothing 2 is supposed to compensate/smooth posture differences as well.  It is Nano smoothing 1 that doesn't look at the rotary motion.

FWIW, smooth TCP is probably the option that would help the most, short of reprogramming with a much finer/smoother input toolpath.

Given the age of the control, I think the key will be creating a very smooth base toolpath.  Focus on smoothing the rotary motion.  The linear movement will be where it is, but generally the smoother the rotary is the smoother the linear motion will be as well.  IMHO, it is almost always best to isolate the jerky motion down to one linear axis at a time.  For me that used to be Z as I used to to wrapped spiral cut parts with a cylindrical or elliptical pattern surface.

[cncappsjames]

@Colin Gilchrist, most of those options you listed are not available on the 18i control.

These options below are probably the most helpful in this instance. You WILL need some servo tuning since most likely none was done with the factory given the age of the control.

NANO Smoothing - A02B-0284-S687

Jerk Control - A02B-0284-S678

AI-NANO HPCC - A02B-0284-S669

 

[Colin Gilchrist]

Yeah, I was going off my 31i-B5 book. I skimmed the original thread, and initially missed that it is an older 18i control.

[crazy^millman]

9 hours ago, cncappsjames said:

@Colin Gilchrist, most of those options you listed are not available on the 18i control.

These options below are probably the most helpful in this instance. You WILL need some servo tuning since most likely none was done with the factory given the age of the control.

NANO Smoothing - A02B-0284-S687

Jerk Control - A02B-0284-S678

AI-NANO HPCC - A02B-0284-S669

 

Trying to help a current customer with a 31iA Control. Seems the B has more parameters than the A and been fighting trying to get G43.4 to work the same as it does on the B control. Odd this is same code for a A Control in a different machine, but same model that run perfectly in that one will not run in this one. G68.2 run perfectly all day long after it was added last month 7 years after they purchased the machine, but now G43.4 is all over the place. Today trying out some code a good friend sent me to see if that is the key for this one odd ball machine to get it running correctly. We have been working on this one for 2 weeks.

[Colin Gilchrist]

15 minutes ago, crazy^millman said:

Trying to help a current customer with a 31iA Control. Seems the B has more parameters than the A and been fighting trying to get G43.4 to work the same as it does on the B control. Odd this is same code for a A Control in a different machine, but same model that run perfectly in that one will not run in this one. G68.2 run perfectly all day long after it was added last month 7 years after they purchased the machine, but now G43.4 is all over the place. Today trying out some code a good friend sent me to see if that is the key for this one odd ball machine to get it running correctly. We have been working on this one for 2 weeks.

Yes, a 31A control is going to be much different than the 31i-B5 unfortunately.

Might need to get Fanuc America involved on this one...

You mention "same code for A Control in a different machine". Any chance you can get a Parameter Dump from the "working machine", so you can compare System Parameters?

 

[crazy^millman]

1 hour ago, Colin Gilchrist said:

Yes, a 31A control is going to be much different than the 31i-B5 unfortunately.

Might need to get Fanuc America involved on this one...

You mention "same code for A Control in a different machine". Any chance you can get a Parameter Dump from the "working machine", so you can compare System Parameters?

Yes I have 10 different parameter dumps from all types of and 4 of the same machines and gone though them with a fine tooth comb and this one machine is just not acting like the others even with the same parameters and control types. We had to get Fanuc involved on a different machine an OKK HM-X6000 and we had to use G68.2 Preposition moves before the G43.4 to get that one working. Previous HM-X6000 machines doing G43.4 never needed it, but that one with the same exact parameters as previous machines wouldn't run the code correctly in G43.4 either. It was only after we got the post changed to Preposition with G68.2 before the G43.4 would the machine work correctly. Then we had two more newer machines needed the same thing. The Builder and Fanuc cannot give solid reasons why and leaving it up to our company and the Machine Supplier to resolve all of this. Hopefully today we get this one resolved and can move on to other paying work.

[crazy^millman]

Update finally got the AE to set everything back to default parameters and start testing things one by one to see which one was the correct setting. Once he did we were finally able to dial it in and get it running without the need for G68.2 before the G43.4. Yeah now we can put this one to bed and more on to paying work.

[cncappsjames]

Myself, I like a G68.2 pre-position. I know it's not necessary and can usually be avoided if desired... I just kinda like it.

[crazy^millman]

9 hours ago, cncappsjames said:

Myself, I like a G68.2 pre-position. I know it's not necessary and can usually be avoided if desired... I just kinda like it.

I don't really care as long as the machine will run what is programmed. The G68.2 preposition is extra code and helps the programmer or machinist have a good idea where a toolpath is going to start, but when you have 50 operations using the same tool I have found the G68.2 before each one takes longer than just hoping between G43.4 and runnign everything all as one section. If the programmer has all the linking and everything else dialed in then no need for the jackhammer effect of sending it home between each 5 Axis operation. That also comes down the experience of the programmer and in some cases how the NC Format or Post is configured. CAMPlete does a good job of allowing things to be controlled once in there, but for MP Post falls back on the programmer to know what the mi and mr switches do to control this behavior.