Question for all you 5th axis experts

[CNC CHRIS]

is there any classes you would recommend to learn multi axis toolpaths?

i know a little bit of multi axis toolpaths but would like to improve. 

i looked at the mastercam website and came across the "Mastercam University : Multi axis toolpahts" course.

is this a good course?

[#Rekd™]

This is on Youtube and he provides the solid models for you to follow along. Great stuff!

 

[#Rekd™]

There is this series with Ron (He is always on this forum helping us!!). Thanks Ron!

 

Then there is Colin (also on here helping us!!!). Thanks Colin!

 

[Shiva.aero]

I recently completed MC University 2021 Multiaxis toolpath course. It is very well organized and have some advanced lessons. The courses on Approximate vs Exact method, Clean core, Stock to focus, etc., are very useful & interesting to learn.

Youtube channels mentioned by Rekd also very informative.

Understanding the Tool axis control strategies and Linking strategies are very important to get good 5 axis toolpath.

Most importantly learn the basics. For example, the default tool axis orientation is the normal direction to the surface and any kind of tilt angle is applied to this direction. Moduleworks documentation will be helpful to know the details. One interesting example I like to share is, for Blade expert application, in Esprit CAM software, the default tool axis orientation is 'surface normal to the blade surface' and whereas in Mastercam it is the 'surface normal to the Hub'. Without understanding this, setting a good tilt angle is difficult and using Collsion control without a good tilt angle will make the toolpath calculation long & worse.

Atlast I suggest to read the related old threads in this forum. Many are gems!

[savagkd]

I'd also add, wherever possible, use 3+2 and pay close attention to your transition between operations.  Most of my problems have happened on the rapid repositions.  Verification software is a must!!!  Vericut has saved my bacon on several occasions.

[motor-vater]

1 hour ago, savagkd said:

I'd also add, wherever possible, use 3+2 and pay close attention to your transition between operations.  Most of my problems have happened on the rapid repositions.  Verification software is a must!!!  Vericut has saved my bacon on several occasions.

Agreed!!! Also if you dont have verification software forced tool changes are like training wheels in 5 axis. Starts from home every toolpath. 5 axis in mastercam seems all good and ez when in verify, but actually verifying G code is a God send, the post plays a significant roll. A misplaced G49 for example will have you polishing up the old resume!!!!!!

[Chally72]

2 hours ago, savagkd said:

I'd also add, wherever possible, use 3+2 and pay close attention to your transition between operations.  Most of my problems have happened on the rapid repositions.  Verification software is a must!!!  Vericut has saved my bacon on several occasions.

Good starting advice, though verification software isn't always necessary depending on machines and scenarios. Generally, motion within the operation is controlled explicitly by the toolpath. Motion between operations (null toolchanges) is controlled by, and varies between, posts. That's where the danger and behavioral mismatch can come in.

[crazy^millman]

52 minutes ago, Chally72 said:

Good starting advice, though verification software isn't always necessary depending on machines and scenarios. Generally, motion within the operation is controlled explicitly by the toolpath. Motion between operations (null toolchanges) is controlled by, and varies between, posts. That's where the danger and behavioral mismatch can come in.

Not always Dylan where kinematic awareness of the programmer needs to come into play. Can program something for a limited travel machine and look good all day in Mastercam and never run on the machine or even crash the machine. Especially one not tied to a post where it does the unwinds and other things that Mastercam from a programming standpoint is never aware of.

[Shiva.aero]

13 hours ago, Chally72 said:

Good starting advice, though verification software isn't always necessary depending on machines and scenarios. Generally, motion within the operation is controlled explicitly by the toolpath. Motion between operations (null toolchanges) is controlled by, and varies between, posts. That's where the danger and behavioral mismatch can come in.

'Motion between operation'

Is it not controlled by 'Multiaxis linking' toolpath?

 

[Colin Gilchrist]

14 hours ago, motor-vater said:

Agreed!!! Also if you dont have verification software forced tool changes are like training wheels in 5 axis. Starts from home every toolpath. 5 axis in mastercam seems all good and ez when in verify, but actually verifying G code is a God send, the post plays a significant roll. A misplaced G49 for example will have you polishing up the old resume!!!!!!

Dude, check Parameter #5006.6 !!!

Bit 6 of 5006, tells the machine to "move" the distance of the TLO when G49 is read, if the value is "0". Set #5006.6 = 1. This tells the control to update the display with the current machine position, without physical motion.

 

This is the first Parameter setting I check when working on any Fanuc control!

If it is set to 1, then you get TLO cancelled without machine motion.

I really can't figure out when this would ever be useful to have it set to '0'.

[Chally72]

12 hours ago, crazy^millman said:

Not always Dylan where kinematic awareness of the programmer needs to come into play. Can program something for a limited travel machine and look good all day in Mastercam and never run on the machine or even crash the machine. Especially one not tied to a post where it does the unwinds and other things that Mastercam from a programming standpoint is never aware of.

Absolutely- no argument there. For someone just getting into 5 axis likely with simple projects on simple machines, I find the additional hurdle of also figuring out an entire 5 axis verification software package at the same time to be a barrier that often may not need to be there.

[crazy^millman]

2 hours ago, Chally72 said:

Absolutely- no argument there. For someone just getting into 5 axis likely with simple projects on simple machines, I find the additional hurdle of also figuring out an entire 5 axis verification software package at the same time to be a barrier that often may not need to be there.

Agree the problem is managers and owners who keep hearing lies from different CAM companies than in 10 minutes of using this certain software anyone can be a full vested 5 axis programmer programming the most complex parts every created and why can't Mastercam do the same thing? Then you have to talk their employees off the ledge because they are being asked why can't they do it in 10 minutes like the salesman selling that lie is saying. I have been programming 5 axis machines of all types for over 20 years and still get my butt kicked on parts. I realize I am normally the dumbest person in the room, but doing something for 20 years should at least give me some idea how and what it takes to do it verses some lie someone is pushing about how this software makes a Walmart greeter by pass all of that just because they purchased said software is all.

[motor-vater]

7 hours ago, Colin Gilchrist said:

Dude, check Parameter #5006.6 !!!

Bit 6 of 5006, tells the machine to "move" the distance of the TLO when G49 is read, if the value is "0". Set #5006.6 = 1. This tells the control to update the display with the current machine position, without physical motion.

 

This is the first Parameter setting I check when working on any Fanuc control!

If it is set to 1, then you get TLO cancelled without machine motion.

I really can't figure out when this would ever be useful to have it set to '0'.

Yes, I might have got that from u in the past, cause it sounds familiar. My problem was the old post would spit out g49's without a g43 after, so it was the Z motion that was called after the g49 that would try to kill the machine, not the TLO call in its self.. Postability was the best money I spent around here... No more wonkie problems like that...

[Colin Gilchrist]

16 minutes ago, motor-vater said:

Yes, I might have got that from u in the past, cause it sounds familiar. My problem was the old post would spit out g49's without a g43 after, so it was the Z motion that was called after the g49 that would try to kill the machine, not the TLO call in its self.. Postability was the best money I spent around here... No more wonkie problems like that...

Ok, that makes total sense Pete. Glad you got hooked up with Postability for quality Post Processors. There is nothing more expensive than a "cheap post".