Multaixis Comp discussion

[Aaron Eberhard]

This is a new thread so we don't clutter up the other thread:

Obviously, most of this (for me) will be about what the NCI does vs. what you want it to do, but as a disclaimer:  The current outputs are based on requests from (and my subsequent followup conversations with) post writers and control manufacturers.  That doesn't mean that I'm saying it's right, but just saying that there is a reason!    That said, this was done over 4 years ago (for me) for release 2018, which means the team actually did the work in early 2017 and I did the research before that, so yeah, it would probably be like real work to dig up the conversations I had with people from then.  And I wouldn't be hanging out on the forum if I wanted to do real work! 

Other disclaimer:  The only multiaxis toolpath that the Left/Right switch actually affects is Curve as far as I know.   Now, the NCI output will have a different value on the 1016 line (parameter #), but the actual contact point & tool position is the same regardless in, say, a flow.   Because of this history, it was requested that the MW toolpaths always just output "Left" on the 1016 line.

All that aside, let's dig into the NCI.  Break your your MP documentation books and play along.

If you look into what a simple contour has for cutter comp info, you'll see something like this

Gcode     NCI    [Contour (2D) - Wear Comp]
G1016     2 10 1 1 0. 0. 0. 41 -1 1 4 0 0. -1 1 1 2 0. 2 1	<--- The "41" means Turn on Left Wear Comp, 42 would be Right>
G-11      START DISPLAY TYPE - Entry
G1        41 -31.65207146 46.3877151 0. 3.58125 2000		<--- The "41" means Turn on Comp>
...
G1        140 -11.65207146 56.3877151 0. 3.58125 200		<--- The "140" means Turn off Comp>
G-12      END DISPLAY TYPE - Exit

Gcode     NCI    [Contour (2D) - Control Comp]
G1016     1 10 1 1 0. 0. 0. 0 -1 1 4 0 0. -1 1 1 1 0. 1 1   <--- No "41/42" at Position #8 means do not coomp left OR right>
G-11      START DISPLAY TYPE - Entry
G1        41 -31.65207146 41.3877151 0. 3.58125 2000		<--- The "41" means Turn on Comp>
...
G1        140 -11.65207146 51.3877151 0. 3.58125 200		<--- The "140" means Turn off Comp>
G-12      END DISPLAY TYPE - Exit

 

Which might be what you'd expect to see on a multiaxis path as well, but in a multiaxis environment, the comp is a whole lot more complicated than it is in 2d.    As a result, it's only been relatively recently that controls even offer it.  What they need is the tool tip, vector (i.e., tip point to 1" or so above the tip to establish the tool tilt vector), but in order to actually comp, you also need to know the tool contact point and the surface normal at that contact point. 

Because of this, our spec for the G11 doesn't even have a callout as to whether comp is on/off.   It's there if the post can use it.  As far as the 5ax toolpath is concerned, comp is always on. 

Let's work through the difference between an old toolpath that has the interface to "turn on" comp, like 5ax Flow on a really simple 5 axis surface and compare all of the comp conditions vs a Morph:

Gcode     NCI    [Flow 5 Axis - Computer Left]
G1016     2 11 45 1 0. 0. 0. 41 -1 1 4 0 0. 0 1 1 2 0. 2 45		<--- The "41" means Turn on Left Comp>
G11       98.74287779 11.84007446 -8.00122507 98.74287779 11.84007446 16.99877493 9.618898 21 0 -0.66728599 -0.52665426 0.52665426 102.74659371 15. -5.16115061
<No code to turn on comp at the beginning, just get right to it.>

Gcode     NCI    [Flow 5 Axis - Computer Right]
G1016     6 11 45 1 0. 0. 0. 42 -1 1 4 0 0. 0 1 1 6 0. 6 45 	<--- The "42" means Turn on Right Comp>
G11       98.74287779 11.84007446 -8.00122507 98.74287779 11.84007446 16.99877493 9.618898 21 0 -0.66728599 -0.52665426 0.52665426 102.74659371 15. -5.16115061

Gcode     NCI    [Flow 5 Axis - Wear Left]
G1016     3 11 45 1 0. 0. 0. 41 -1 1 4 0 0. 0 1 1 3 0. 3 45
G11       98.74287779 11.84007446 -8.00122507 98.74287779 11.84007446 16.99877493 9.618898 21 0 -0.66728599 -0.52665426 0.52665426 102.74659371 15. -5.16115061

Gcode     NCI    [Flow 5 Axis - Wear Right]
G1016     5 11 45 1 0. 0. 0. 42 -1 1 4 0 0. 0 1 1 5 0. 5 45
G11       98.74287779 11.84007446 -8.00122507 98.74287779 11.84007446 16.99877493 9.618898 21 0 -0.66728599 -0.52665426 0.52665426 102.74659371 15. -5.16115061

Gcode     NCI    [Flow 5 Axis - Control Left]
G1016     9 11 45 1 0. 0. 0. 0 -1 1 4 0 0. 0 1 1 9 0. 9 45		<--- No Comp call out with Control comp>
G11       98.74287779 11.84007446 -8.00122507 98.74287779 11.84007446 16.99877493 9.618898 21 0 -0.66728599 -0.52665426 0.52665426 102.74659371 15. -5.16115061

Gcode     NCI    [Morph]
G1016     7 11 442 1 0. 0. 0. 41 -1 1 4 0 0. 0 1 1 7 0. 7 442	<--- The "41" means Turn on Left Comp>
G11       99.73387532 11.53055837 -7.04837039 99.73387532 11.53055837 -1.04837039 9.618898 20 0 -0.67107089 -0.52424415 0.52424415 103.76030068 14.67602327 -4.19383529
<No code to turn on comp at the beginning, just get right to it.>

So you can see that if your comp is working correctly with Flow, it should be working correctly with Morph.

 

That said, if we're missing something that you guys need, please let me know!  It was implemented this way based on the requests from some control manufactures after consulting with various post guys.

[crazy^millman]

Great now that we have that out there. What about the new Swarf where we would want to control left or right? I might 5 Axis a surface one way with a Ball endmill and if I had Left G41.5(G41.2) and Right G42.5(G42.2) control then I could 5 Axis 3D adjust that shape along that shape with 5Axis Comp either way where as what your saying is we are forced into one direction because the default is left only. Sometimes on some material conventional cutting is better verses climb and in those cases having Right Comp ability would be required not left only comp ability. On full bidirectional cutting you are correct not really a difference and we would use just the G43.8 process that takes the vectors into account as it adjust the tool bidirectional along the cut, but in places where want one directional adjustment in 5 Axis we currently don't have a mechanism for controlling that output like we do in the old school toolpaths.  4 years ago this was added for NCI output, but not in the MW toolpaths where a lot has been done to make them more user friendly. Is asking for a controlled process for direction when users want them really that hard to have added? 

What Generic post is supporting this output for 5 axis machines? What MT has this supported? Where in MT can I tell it to output the 5 Axis comp? 

[Aaron Eberhard]

20 minutes ago, crazy^millman said:

Great now that we have that out there. What about the new Swarf where we would want to control left or right? I might 5 Axis a surface one way with a Ball endmill and if I had Left G41.5(G41.2) and Right G42.5(G42.2) control then I could 5 Axis 3D adjust that shape along that shape with 5Axis Comp either way where as what your saying is we are forced into one direction because the default is left only. Sometimes on some material conventional cutting is better verses climb and in those cases having Right Comp ability would be required not left only comp ability. On full bidirectional cutting you are correct not really a difference and we would use just the G43.8 process that takes the vectors into account as it adjust the tool bidirectional along the cut, but in places where want one directional adjustment in 5 Axis we currently don't have a mechanism for controlling that output like we do in the old school toolpaths.  4 years ago this was added for NCI output, but not in the MW toolpaths where a lot has been done to make them more user friendly. Is asking for a controlled process for direction when users want them really that hard to have added?  

What Generic post is supporting this output for 5 axis machines? What MT has this supported? Where in MT can I tell it to output the 5 Axis comp? 

That's not exactly what I'm saying, what I was saying is that I've yet to see a control spec where you can do a multiaxis axis comp as "left or right."   It's not like a 2 axis spec.  In your swarf example, it's going to be comped the exact way a parallel would be.   The fact that it's a swarf is kind of irrelevant.  A Swarf is just a parallel (or flow or...) leaned over 90°. 

I don't believe any generic posts support this, but I'm not sure.  I'm not really a post guy

I don't know what MT machines support this, either.    If memory serves, I was only able to find 3 or 4 controls that even had 5 axis comp and only two manufacturers got back to me, the other source was from our post partners.

20 minutes ago, crazy^millman said:

Is asking for a controlled process for direction when users want them really that hard to have added?  

I don't believe that this is the right tone to take with the discussion, and I hope that the tone of this statement is not what you were really intending. 

No, obviously adding a switch in the software would not be hard, but even if there was a switch, there's no spec in the multiaxis toolpaths to DO anything with that switch.   It doesn't do anything in the Flow, Msurf, or any other surface-based toolpath, either.    It can do something with Curve because curve doesn't need a surface to work and it will just change the calculation point on the chain.  Other than Curve, does anyone have any examples they can send in of that switch being used?

If you have some sort of new information about how the controls that you work with can support multiaxis tool comp, please send it over.  Previously there really wasn't any info provided by the control manufacturers, and as far as I know the post writers just ran with it.   There has been very little feedback, but the previous discussion showed there was obvious desire from a few people which is the purpose of this thread. 

The point here is to figure out exactly what you guys are missing out on so I can either update the interface & toolpaths if necessary, and/or give it to the post team to expand the NCI definition of the G11 (Multiaxis) moves.

[Guest]

5 minutes ago, Aaron Eberhard - CNC Software said:

No, obviously adding a switch in the software would not be hard, but even if there was a switch, there's no spec in the multiaxis toolpaths to DO anything with that switch.

 Logically, the way I see it an additional line would have to be added to the NCI from Mastercam with the result of the switch

Then it would be up to the post developers to do something with that data.

[crazy^millman]

50 minutes ago, Aaron Eberhard - CNC Software said:

I don't believe that this is the right tone to take with the discussion, and I hope that the tone of this statement is not what you were really intending. 

Sorry you think my tone is off.  I thought it was pretty chill in the request, but seems as though it is not coming across that way. It was done last week and I was asking for then that would be pushing it, but after 4 years of having the option asking for it I thought was a pretty fair question.

I have some Beta testing to do with one of the post builders on this very subject with a few different controls and machines. It will be a 3 to 6 month process to go through them. Once I have collected that information and can provide solid real world examples of where, how and when what I am envisions can be used I will share it like I always do with QC and make sure to copy you at that time. If I am wrong like I am from time to time then I will come back and admit I was totally off in my thinking and method that using this can and should be implemented.

For now I have said my peace and hopefully others will have something else to add to further the conversation along in a constructive and productive way. Thank you for taking the time to have a conversation about it and have a good day.

[cncappsjames]

My request is quite simple;

Give us comp selections just like the old school Flow 5-Ax, Curve 5-Ax, and swarf. 

Easy peasy, lemon squeezy, then set/flag the condition in the NCI. 

That's it. 

[#Rekd™]

19 hours ago, Aaron Eberhard - CNC Software said:

I don't believe that this is the right tone to take with the discussion, and I hope that the tone of this statement is not what you were really intending. 

Not speaking for others but I thought the discussion was constructive with tons of possibility for further enhancements.

All good thoughts here and I am glad you are here Aaron trying to help!

[Elvincnc]

@Aaron Eberhard - CNC Software What tool path(5 axis) support contact point, surface vector. The more data we have, the more opportunities

Some Nx users are able to output 3D tool compensation for different controls, having a macro language cnc 

https://onedrive.live.com/?authkey=!AA1qEKjCBhcZ0bQ&cid=5253BAA9395B721F&id=5253BAA9395B721F!12388&parId=5253BAA9395B721F!7462&o=OneUp

 

 

 

[Guest]

7 minutes ago, Elvincnc said:

What tool path(5 axis) support contact point, surface vector

He answered that on the other topic, 

"Any (CNC or MW) multiaxis toolpath that deals with surfaces will output the tool center point, tool vector, surface contact point, surface normal at the contact point, and all of the contour flags are accurate."

[Metallic]

3 hours ago, #Rekd™ said:

Not speaking for others but I thought the discussion was constructive with tons of possibility for further enhancements.

All good thoughts here and I am glad you are here Aaron trying to help!

I would also agree.

To the other posters points, it is 100% safer and easier to modify something you want to do from within the parameters window via dropdown/selection vs having to modify NCI data or mess with posts to get output that may or may not be what is desired. Lots of things can go wrongly during that process...

Process reliability is very important.

 

For example, Im running a custom heat sink on my 5 axis mill. I had the machine crash recently (nothing bad luckily) because the PLANES are STILL messed up. I had to go back into all my ops and clear the planes to TOP and reset them. This bug has been brought up before with CNC software and it still hasn't been resolved. IDK what the planes are doing, but it creates a tool vector that makes no sense. So instead of positive Z values on your tilted workplane, your code is negative Z values.

Im guessing none of us want to hear the sound of a spindle rapiding at 100% THROUGH your trunnion....but yet that is almost what happened.

[huskermcdoogle]

18 hours ago, cncappsjames said:

Give us comp selections just like the old school Flow 5-Ax, Curve 5-Ax, and swarf. 

Easy peasy, lemon squeezy, then set/flag the condition in the NCI. 

I think I start to stand with Aaron on this one a little.  It's not so easy....

I suppose having a switch would be easy, but I am starting to understand why left/right is irrelevant on a surface based path.  Technically speaking if you are comping to a surface normal vector as you would with "true" 5axis comp then left/right doesn't have any bearing whatsoever because the resulting comp vector will dictate the direction.  but if you aren't feeding the machine the comp vector than the "side" becomes relevant assuming a wear offset.

Fascinating subject.

I think we need to start breaking this down into sub sets.  Specific comp types for specific toolpath types and shapes, on a specific control.  I would say if we want to get serious about helping develop new practices or standards moving forward we will need to start making sure we are all talking apples to apples.

Basically speaking, as I understand it, there are two types of comp:

Side Comp (in a plane normal to the tool axis) - This would typically be done on a Fanuc with G41.2/G42.2.  This would typically be applicable for say a curve 5x, or a swarf path, but less likely to be used with morph or parallel.  I can see zig/zag cuts with swarf being a challenge if were to just set G41.2 and roll on.   I think you would want it to flip the comp direction at the link between slice.

Surface Comp (in the direction of the surface normal for use with ball nose or bull nose on free form surface) - This would be used with say Morph, Parallel, and so on and would be more for use ball nose cutters. This is where Left/Right wouldn't really be applicable here as the vector would control the direction.  I don't have any experience with this type of comp, so please, those that do, chime in.

[crazy^millman]

46 minutes ago, huskermcdoogle said:

I think I start to stand with Aaron on this one a little.  It's not so easy....

I suppose having a switch would be easy, but I am starting to understand why left/right is irrelevant on a surface based path.  Technically speaking if you are comping to a surface normal vector as you would with "true" 5axis comp then left/right doesn't have any bearing whatsoever because the resulting comp vector will dictate the direction.  but if you aren't feeding the machine the comp vector than the "side" becomes relevant assuming a wear offset.

Fascinating subject.

I think we need to start breaking this down into sub sets.  Specific comp types for specific toolpath types and shapes, on a specific control.  I would say if we want to get serious about helping develop new practices or standards moving forward we will need to start making sure we are all talking apples to apples.

Basically speaking, as I understand it, there are two types of comp:

Side Comp (in a plane normal to the tool axis) - This would typically be done on a Fanuc with G41.2/G42.2.  This would typically be applicable for say a curve 5x, or a swarf path, but less likely to be used with morph or parallel.  I can see zig/zag cuts with swarf being a challenge if were to just set G41.2 and roll on.   I think you would want it to flip the comp direction at the link between slice.

Surface Comp (in the direction of the surface normal for use with ball nose or bull nose on free form surface) - This would be used with say Morph, Parallel, and so on and would be more for use ball nose cutters. This is where Left/Right wouldn't really be applicable here as the vector would control the direction.  I don't have any experience with this type of comp, so please, those that do, chime in.

Okay and we want 5 Axis Comp output or we don't. What comes from the MW toolpaths to the post as a Flag for that? That is all I am asking for. Make a switch in them to use it or not integrated into the operations.

I think you are correct there are 2 types of comp, but as I said if I was going one way with a 5 Axis toolpath and the geometry was such where using left or right allowed it then it would be cool to invoke it. Now will full 5 Axis comp do the same thing in that situation it might.

Then what is also happening in the some of the Old School toolpaths has been wrong for a long time and no one has ever addressed that issue. If the Left and Right serve no purpose in some of the 5 Axis toolpaths when they were added originally to the software that was an error is the other part of the discussion that has come out of this conversation. It happens and not a point a finger comment, but an observation this conversation has brought to light. I don't do mold work anymore and majority of the work I do is always understood replace the tool if it is getting wear on it. That is not the rest of the world and people use regrinds and people push tools past the breaking point trying to get that extra 5 minutes of cut out of it. Nature of what we do and if the machines have the capability built into them to allow people the ability to use it then putting the methods in the software to support it is part of the process in developing software. If it were not something people wanted then it would have never got added for output in 2018 with the G11 addition. Currently what sends this flag to the post from the MW toolpaths to use 5 Axis Comp or not use it? Nothing I am aware unless a post builder adds a switch to make it happen. The old school toolpaths do have a flag from them integrated in the operations and working. If that is 100% correct or not it is still is a part of them. If asking for MW toolpaths to do the same thing is not going to happen then okay. I have been told no many times over the years about things in the Software only to see them show up years later and how do we progress the process? We ask questions push the envelope and try. Do we always get it right the 1st time? 2nd? 3rd? 20th? No, but willingness to keep trying has to happen and that is what I push myself and others to do.

[Chally72]

It's definitely not a simple topic- I can't articulate exactly what I would want and I'm an "end user" here, in a lot of respects. Just my own thoughts- anything that is added as far as interface has to be maintained and get the buy-in of post developers to actually implement. Otherwise, it's a dead switch in the software that does nothing and can't tell you it does nothing because it has no idea if your post supports it or not. Beyond a simple Comp On/Off switch, I truly don't know what I would ask for. As mentioned, left/right or reverse wear/control don't really have initial bearing here. There is also already the tip/center switch for toolpath calculation.

[Aaron Eberhard]

@Elvincnc - Thanks for those videos, looks like I'm heading down another rabbit hole    Any idea what the codes are for that it's simulating?   Looks like it would be for a Siemens 840 or something, but I haven't found R810/R811/R825 parameters in the manuals I've found for those online which are the parameter's he's manually editing in the beginning of the first video. 

----------------------------

On 2/18/2021 at 1:19 PM, Thee Byte™ said:

 Logically, the way I see it an additional line would have to be added to the NCI from Mastercam with the result of the switch 

Then it would be up to the post developers to do something with that data. 

The problem that I'm having is that I can't find any specs more than what I've previously received ("just make sure that the toolpath has the contact point and surface normal and we'll deal with it").  Do you have any specific needs (i.e., I need to turn on the comp code (whatever that is) at the beginning of the file, after the null tool change. Or is it more of a We need this after every linking move).

----------------------------

@crazy^millman Yeah, I wasn't interpreting it as negative, but I did view that comment and this one from James as unnecessarily flippant, as neither adds anything to the conversation:

22 hours ago, cncappsjames said:

My request is quite simple;

Give us comp selections just like the old school Flow 5-Ax, Curve 5-Ax, and swarf. 

Easy peasy, lemon squeezy, then set/flag the condition in the NCI. 

That's it.

I don't think this is that simple.   It doesn't answer the question of "what's different between the "good" toolpaths (e.g., CNC Flow) and the "bad" toolpaths (e.g. Morph)? " As I demonstrated in my original post, they're exactly the same output, so how are you guys using them differently?   Is Flow good and Morph bad because it has a switch in the interface that seemingly doesn't do anything?

Ron's second post looks like it will yield much more helpful information

----------------------------

To boil it down to the actionable question;  With the understanding that this was implemented as requested by the control and post guys who sent it over to me (as I am not a post guy!), what options do you need to see in the interface (check box to turn comp on/off?, pull down with "left/right/wear/control/etc), and what exactly do you want to see in the NCI that you're not seeing now?

----------------------------

Thanks to everyone in the conversation!

[Aaron Eberhard]

4 hours ago, huskermcdoogle said:

I think I start to stand with Aaron on this one a little.  It's not so easy.... 

I suppose having a switch would be easy, but I am starting to understand why left/right is irrelevant on a surface based path.  Technically speaking if you are comping to a surface normal vector as you would with "true" 5axis comp then left/right doesn't have any bearing whatsoever because the resulting comp vector will dictate the direction.  but if you aren't feeding the machine the comp vector than the "side" becomes relevant assuming a wear offset.

Fascinating subject. 

I think we need to start breaking this down into sub sets.  Specific comp types for specific toolpath types and shapes, on a specific control.  I would say if we want to get serious about helping develop new practices or standards moving forward we will need to start making sure we are all talking apples to apples. 

Basically speaking, as I understand it, there are two types of comp:

Side Comp (in a plane normal to the tool axis) - This would typically be done on a Fanuc with G41.2/G42.2.  This would typically be applicable for say a curve 5x, or a swarf path, but less likely to be used with morph or parallel.  I can see zig/zag cuts with swarf being a challenge if were to just set G41.2 and roll on.   I think you would want it to flip the comp direction at the link between slice. 

Surface Comp (in the direction of the surface normal for use with ball nose or bull nose on free form surface) - This would be used with say Morph, Parallel, and so on and would be more for use ball nose cutters. This is where Left/Right wouldn't really be applicable here as the vector would control the direction.  I don't have any experience with this type of comp, so please, those that do, chime in.

Sorry to corrupt you

 

For all practical purposes, Swarf needs to be treated as any other surface-based toolpath (pretend it's parallel with 90° side tilt).  Whether you're driving off of wireframe or surfaces, you're drawing a line between the two rails, and that's your contact "point."  Regardless of direction, you need to comp normal to that contact "point" or your comp would be incorrect.   It's actually remarkably similar to the problem that Swarf has with collision control/de-gouge behavior. 

Curve is the only toolpath that can truly be ran without any surface, so as this discussion reveals, that's the only one that should keep the "left/right" option.   

The other question is what value is the "Computer/Control/Wear/Reverse Wear/Off" has to any of these?

[huskermcdoogle]

1 hour ago, Aaron Eberhard - CNC Software said:

The other question is what value is the "Computer/Control/Wear/Reverse Wear/Off" has to any of these?

After thinking about this more today, what I think it really boils down to is the ability to at least turn it on and off.

I also think it would be nice for many people to be able to use it on swarf, but maybe only in one way mode, or if in zig/zag would give you the ability to flip when going in the conventional direction.  It would make it such that you don't need to use vector based comp.  The machine can and will compensate on it's normal to the tool axis and toolpath direction, which in the case of a cylindrical tool would be the same as the contact point normal vector.

What I would like to know, is that if you have G41.2, do you automatically have G41.6 (type 2 vector based comp) on a Fanuc?  Maybe this is something James or Ron can chime in on.  But I think at some point here we need to get some good use case info in place.

I know for me personally, I had two use major cases.  One for where I wanted to run regrind endmills and was using 5x curve, as well as standard contour paths without G68.2,  And one where I was doing rotary surfacing where I had the need to run an 80mm ball with reground blades.  This is where I would have needed vector based comp, but at the time I didn't have the time to modify my post to transform the surface contact point data to match the machine kinematics.  Not even on a test basis.  Therefore I was never able to test vector based comp on the machine.  I used to program everything from the center of the radius, so it wouldn't have been a problem to just update offsets and let it fly.  I had a large pile of dull blades and a big need for using them.  So my solution ended up being to have .25mm different increment programs, and run them when I was running abrasive laminate materials.  Not a big deal.  But comp also would have been useful for making size adjustments that don't effect other features, without having to change work offsets in relation to center of rotation.   In this case we were not using TCP for the table rotary axis, but we were using it for the two head rotaries, so there was that complication as well.

[crazy^millman]

1 hour ago, huskermcdoogle said:

After thinking about this more today, what I think it really boils down to is the ability to at least turn it on and off.

In a Nutshell that is what I am saying.

[cncappsjames]

9 hours ago, huskermcdoogle said:

Basically speaking, as I understand it, there are two types of comp:

Side Comp (in a plane normal to the tool axis) - This would typically be done on a Fanuc with G41.2/G42.2.  This would typically be applicable for say a curve 5x, or a swarf path, but less likely to be used with morph or parallel.  I can see zig/zag cuts with swarf being a challenge if were to just set G41.2 and roll on.   I think you would want it to flip the comp direction at the link between slice.

Surface Comp (in the direction of the surface normal for use with ball nose or bull nose on free form surface) - This would be used with say Morph, Parallel, and so on and would be more for use ball nose cutters. This is where Left/Right wouldn't really be applicable here as the vector would control the direction.  I don't have any experience with this type of comp, so please, those that do, chime in.

Correct IMHO.

Re: Ball/Bull... I'll preface this statement by saying I would never do this, however, I recently lost a battle with a customer regarding + Tool Lengths (they elected to run negative tool length offsets on their 5-Axis machine so it can be like all their other machines in the shop - no judgement other than they are really missing out but, they have to work with their 4 walls and I do not), so, there are ALL kinds of practices out there. Some sound, others... not so much.

I guess the bottom line is I'm just going to need to work though the tool offset table R/D G/W and CR G/W then

Swarf_Flow_Curve-01.txt

Swarf_Flow_Curve-02.txt

Swarf_Flow_Curve-06.txt

*-01 is New School Swarf - Side Autodetect

*-02 is Old School Swarf Wear

*-06 is Old School Computer

Seems like there is no shutting G43.8 off from the toolpath itself. Good thing I can from within CAMplete.

[Elvincnc]

13 hours ago, Thee Byte™ said:

Any (CNC or MW) multiaxis toolpath that deals with surfaces will output the tool center point, tool vector, surface contact point, surface normal at the contact point, and all of the contour flags are accurate.

MP Doc. 2020 - xsrf$, ysrf$, zsrf$ The X, Y, and Z coordinates of the tool contact point.
This data is only supported for certain multiaxis toolpaths:
Curve 5-axis (tool_op $ value 29), Swarf (tool_op $ value 48), Multisurf (tool_op $ value 110), Flow (tool_op $ value 45), Port (tool_op $ value 112)Surface normal vector (p_svec$, q_svec$, r_svec$). These are used for 3-axis cutter compensation. They are the surface normal at the current tool position with NCI Gcode 11 data.

[Elvincnc]

@Aaron Eberhard - CNC Software Part of the code is calculated in the postprocessor from the data and is output to variables for calculating wear already in the program test.NC

I think they have a motion vector, because the most difficult thing is to get a transition from a flat to a sloped surface or radius

[Newbeeee™]

Interesting thread and shows (to me) what a different world from the 3/4axis world the 5ax world is...

 

[huskermcdoogle]

@Elvincncthat code is interesting.  The only thing that I see as an issue with it is that you wouldn't be able to run it in AICC as IIRC you can't have macro code when in lookahead mode on a Fanuc.  Stupid I know, but that is how it is...  Otherwise that is a great way to be able to adjust the program output for tool variation without having to go back to the CAM system or without having the 3axis comp option on the machine control.

[cncappsjames]

2 hours ago, huskermcdoogle said:

@Elvincncthat code is interesting.  The only thing that I see as an issue with it is that you wouldn't be able to run it in AICC as IIRC you can't have macro code when in lookahead mode on a Fanuc. .....

You caaaaaaaaaaaan however it does require some extra work on the front end to stop the look ahead to make certain the calculations happen. Some machines have a buffer stop M-Code set/created from the factory. Others do not. In the machines that do not, one has to be created and assigned. Not a big deal if somebody knows how to do that, REALLY problematic if they don't.

The average 3/4-Axis user probably thinks many of us are just being a PITA for harping on the issue(s) above. That's fine, this isn't their world... today. However, if things continue as the industry anticipates it will, this will soon be their world so paying attention and learning would be in their best interest. I say that because the number of 5-Axis machines getting delivered increases every single year. In my 16 years at the company I am at, we've only had 2 years where that didn't hold up. 2009 and 2010.

Situations/conditions like this are why Applications Engineers exist.

[crazy^millman]

1 hour ago, cncappsjames said:

You caaaaaaaaaaaan however it does require some extra work on the front end to stop the look ahead to make certain the calculations happen. Some machines have a buffer stop M-Code set/created from the factory. Others do not. In the machines that do not, one has to be created and assigned. Not a big deal if somebody knows how to do that, REALLY problematic if they don't.

The average 3/4-Axis user probably thinks many of us are just being a PITA for harping on the issue(s) above. That's fine, this isn't their world... today. However, if things continue as the industry anticipates it will, this will soon be their world so paying attention and learning would be in their best interest. I say that because the number of 5-Axis machines getting delivered increases every single year. In my 16 years at the company I am at, we've only had 2 years where that didn't hold up. 2009 and 2010.

Situations/conditions like this are why Applications Engineers exist.

Also 5th Axis programming and consulting people like myself. 

[Aaron Eberhard]

On 2/20/2021 at 1:22 AM, Elvincnc said:

MP Doc. 2020 - xsrf$, ysrf$, zsrf$ The X, Y, and Z coordinates of the tool contact point.
This data is only supported for certain multiaxis toolpaths:
Curve 5-axis (tool_op $ value 29), Swarf (tool_op $ value 48), Multisurf (tool_op $ value 110), Flow (tool_op $ value 45), Port (tool_op $ value 112)Surface normal vector (p_svec$, q_svec$, r_svec$). These are used for 3-axis cutter compensation. They are the surface normal at the current tool position with NCI Gcode 11 data. 

I don't have old versions of the manual handy, but the new one definitely says

Quote

The variables xsrf$, ysrf$, and zsrf$ represent the X, Y, and Z coordinates of the tool contact point. These coordinates represent the location on the surface of the part that is in actual contact with the tool. This data is typically used to support 3D cutter compensation. If the tool axis vector is normal to the surface (and the lead/lag angle is 0), this location will be the same as the tip of the tool.

xsrf$, ysrf$, and zsrf$ are supported for any multiaxis toolpaths that work with surfaces. For any unsupported operations, the NCI 11 line will have values of (0, 0, 0) for xsrf$, ysrf$, and zsrf$.

This data was added for Mastercam 2018.

So I'm guessing the post documentation team caught up at some point in the past year or two.  

 

On 2/20/2021 at 1:34 AM, Elvincnc said:

@Aaron Eberhard - CNC Software Part of the code is calculated in the postprocessor from the data and is output to variables for calculating wear already in the program test.NC

I think they have a motion vector, because the most difficult thing is to get a transition from a flat to a sloped surface or radius

Oooooh, I get it now..  Thanks for giving the sample of code.  So 810/811/825 a local memory position, which is why I couldn't find it defined in the manuals the other day!  I didn't quite catch that you literally were manually updating the NC file   So all of the comp is calculated locally, Neat!