MasterCam 3d compensation?

[Tedarencn]

Hi, Guys

 

Does someone knows MasterCam have 3d compensation option?

 

Thanks!

[crazy^millman]

3d compensate what? Code or a model? What specific information are you looking for?

[JoshC]

I believe with 3d Comp you will need the IJK vector for every single position of code, this IJK vector is used by the machine for comp direction and correct me if I am wrong but only the multi-axis toolpaths will relay that info to the post processor.

Unfortunately that's all I know about 3d comp so far, I am hoping to learn more too on this subject so hopefully we get some others that can chime in and give us more detailed info.

[brandon b]

There's a 3d comp chook. Never used it but I remember seeing it in there

[JoshC]

Not a chook, this topic is in regards to 3d CNC cutter compensation for a 5 axis cnc machine. I was hoping we would get some feedback from someone at CNC software, can you let us know if there are in fact certain multi-axis toolpaths that will support 3d compensation? obviously the post processor would need to support the function as well but I am wondering if like a triangular mesh or like a morph between curves would support something like this.

Here is a video I found showing 3d comp for those who are unfamiliar, I am not sure how many machines are supporting this yet but I know some of the newer makinos have this option.

[Colin Gilchrist]

Hi Josh,

 

There are really two types of compensation available for 5X machines, from a "machine" perspective.

 

• Many modern controls support "5X compensation", which is typically a "G41.x" and "G42.x", where the "x" can be .2, .3, .4, .5, or .6, depending on which "mode" is being used. (Typical would be G41.2, G41.4, or G41.5). These "modes" allow the machine's control unit to look at the position vectors that are being output, and using "look ahead/behind" algorithms, the control will offset the cutter position left/right to compensate for a change in tool size. So you can take a .500 diameter cutter, and enter .492 or .530 (or any +- value really), and the control will offset the "path" left or right, based on the "size" of the compensation parameter. This happens "internally" inside the control, and depending on the "mode" you are using, will allow left/right, or will allow you to comp a "corner radius", with a mode like "leading edge offset".
• When using this type of 5X compensation, the only real modification that needs to be done is to modify the post processor to output the correct "5X compensation code", when Control, Wear, or Reverse Wear is selected in the Tool Path parameters. The only paths that support this output currently are the "Original" 5X paths, produced by CNC Software. This would be Curve 5X, Flow 5X, Swarf 5X, and MSurf 5X.
• The other type of "3D compensation" is done with Ball Endmills (only). When using this "3D Comp" option, you are typically outputting the "Center" point of the ball endmill in your NC code, and the machine will offset this position by the Compensation Radius value. When you look at the code output, you typically output "XYZ" coordinates, and also output a "compensation vector" (UVW), which tells the machine "what direction" to offset the path, to comp for the size of the ball endmill.
• Haas for example, uses G141 to invoke 3D comp.
• The 5X paths (NCI Gcode 11) already contain the "Surface Normal Vector" in the NCI data. So it is a pretty simple post modification to "turn on 3D comp mode", and just output the additional UVW vector on the "G1" line.
• Any of the "Surface Finishing" paths (3D tool paths) can be "converted" into output that supports 3D compensation. This is done by programming the path using a normal 3D tool path (say Flowline, or Surface Finish Contour), and then running the "3D Comp" C-Hook. This converts the "normal" (G1, G2, G3) path code into "G11" moves, and writes the additional "Surface Normal Vector" info to the "G11" line. This allows you to compensate for different sized Ball Endmills. (It only works on Ball endmills, as far as I know.) You can play around with the options (Surface Contact Position vs. Tool position). I've always used "Surface Contact Position", although the Help file mentions doing it the other way round...

 

As far as I know, none of the ModuleWorks Multi-Axis Tool Paths support 5X Compensation output. (There is no drop-down list for choosing "computer", "control", "wear", or "reverse wear" options)

 

I believe you can overcome that limitation by using a Misc. Integer or Real Number to trigger the proper output in the post processor. The real question in my mind is; what type of compensation (3D or 5X) are you after?

 

Many people really want "5X Comp", so they can shift the tool left/right on the path.

 

Others want "3D Comp", because they are finishing surfaces like a mold cavity, and they either want to comp to the actual tool size of the ball, or they want to account for tool wear during the machining process. So as the programmer creates a finish path, they may wish to make "incremental" adjustments to the ball radius. Say you were finishing a large mold cavity, you might want to make a .0001 adjustment to the ball radius, at several places along the path. This could be accomplished by breaking up the path into several operations, and making an adjustment (either manually by changing the offset, or automatically, using a G10 line).

 

Regardless of which "method" of comp you ultimately desire, some post processor modification are necessary...

 

Best regards,

 

Colin

 

 

 

 

 

 

 

 

All of the "Multi-Axis" paths,

[JoshC]

Thanks a bunch Colin, that is very helpful information and I appreciate you taking the time to write it up.

[huskermcdoogle]

So I have been looking into adding 3d comp into my multiaxis post.  We are talking G41 with IJK vector of compensation on each block, not a g41.x .  At least this is what code I believe I need to use....  at this point I am fine with the post modifications to get this done, I believe I can get it done without too much hassle.  My issue is mostly with on the Toolpath side of things and the surface normal position.  It appears that the surface normal position that is generated will only be on the pattern surface.  So, like in most cases of my programs I am using a pattern surface and compensating to other surfaces using collision control in the moduleworks paths, or compensation surfaces in the moduleworks paths.  To generate code that will run on the machine efficiently, using a cylindrical pattern surface is about the only choice, this way movement is pretty much forced to one rotary and one linear axis at a time.  Adding two linear just adds problems as the whole bridge needs to move.   Much much slower and far more violent / hard on the machine think, head/head router with rotary table along x as well.  So to finish this thought, I don't believe I can get the surface contact normal for the surfaces I need to compensate to.  Might this be a bug, limitation, or is there something that I am missing here?

 

Husker

[David Colin]

Did you mean this (from MP documentation) is outputting pattern surface normals instead of compensation surface normals?. So i guess it should be considered as a bug because it's useless for what it's been deisgned for...

 

 

p_svec$  q_svec$  r_svec$

 

Category Cutter compensation
Description Surface normal vector.

These numeric variables are for 3-axis cutter compensation.
They are the surface normal at the current tool position with NCI
Gcode 11 data.

[huskermcdoogle]

That's the way I look at it.  We will have to see if anyone jumps on this train with us.

[Matthew Hajicek - Singularity]

Very informative Colin, thank you.

[Colin Gilchrist]

It's not a bug. The paths work as designed. The Comp Vector is relative to the pattern surface.

 

Those 'compensation' surfaces (in the MW paths) are part of their "collision avoidance" strategies. Take the option to "retract along tool axis" as an example. That strategy is not looking at the normal vector of you compensation surface. It is simply retracting the tool until the algorithm finds the tangent contact point of the tool.

 

ModuleWorks would have to add a new algorithm to then take that contact point of the cutter and project it normal to the compensation surface it is tangent to.

 

If you want 3D comp, use a 3X path, in 3 + 2, and run the 3D Comp Chook. Or use one of the old school 5X paths, where your pattern/comp surfaces are the same thing.

[huskermcdoogle]

FYI same result with old school multisurf path.  Still goes to the pattern surface, not the compensation surface.  I don't look at this per say as a bug, just a major limitation in the software that should be addressed, as I am sure many of us would love to be able to use 3d comp with a ball mill on with our 5ax toolpaths.  Is it needed all the time? No.  But would it help those of us that do production runs with 5ax surfacing? Certainly.  I am sure it would be easy for the moduleworks team to give a setting to output to one or the other depending on our needs, they already know the tangent point, it would just be a matter of the transformation of that point and converting it to a unit vector and then writing outputting to the nci accordingly.  Of course I simplify that, but all of the framework needed is there, just a matter of manipulating it and outputting it.

[Colin Gilchrist]

I agree it would be useful, but I think you might be overestimating how many people want 3D comp with 5X surfacing. Probably less than 1% of the users would use it. 5 Axis Comp is much more useful in my opinion, but it really depends on the type of work you do. If you are making Molds, then sure. If you have to blend tools together, absolutely, but those users are the top of the heap.

 

I also think it would be easy for someone to add this as an enhancement. The issue is always the allocation of precious resources. If someone is adding this feature, then they are taking away from something else. I don't mean to be pessimistic about it, but I find that whatever request is getting the most votes usually wins...

[Guest]

I use it... CAMplete puts out G41.2/G42.2 when I use wear comp on 5-Axis toolpaths. :

 

FWIW, the new awesome 5-Axis toolpaths REMOVED CUTTER COMP  therefore I do not use them.

[Newbeeee™]

 

 

FWIW, the new awesome 5-Axis toolpaths REMOVED CUTTER COMP  therefore I do not use them.

I guess that's the price of progress...

[huskermcdoogle]

I wonder how many people would use it if it was readily known how to use it?  More machines shipped these days have lots of options like these turned on, but they aren't taking advantage of what they already have.  For example I hadn't known what I had for options until I started comparing the manual to the fanuc data sheet.  Turns out making hand edits to things on the fly are pretty darn easy one you start throwing things in there like G68.3 and the lot.  I constantly have had the need to just make quick "safe" tweaks to simple drilling routines, or need to make size or blend adjustments due to thermal drift (40-50 degree swing in the shop sometimes).  I can't be the only one in that boat.  I think it just comes down to education, and knowing how to apply some of these advanced functions on the machine.  Thanks for confirming that I am not crazy and missing something, it's much appreciated, I will see about having my re-seller put in an enhancement request.

[huskermcdoogle]

I use it... CAMplete puts out G41.2/G42.2 when I use wear comp on 5-Axis toolpaths. :

 

FWIW, the new awesome 5-Axis toolpaths REMOVED CUTTER COMP  therefore I do not use them.

 

 

I use G41.2/G42.2 regularly with square ended tools for contouring.  Very handy, both when doing toolplane paths on a head head machine, for for 5ax contour cuts, certainly makes life easy.

[Guest]

Husker, sadly the majority of AE's in the US are inadequate. That's just the reality. Sometimes I think most of them are just too effing lazy to learn. Too lazy to pick up a manual. Too lazy to puck up a phone. Then there is the customers that don't know what they don't know.

 

I always do my best to teach my customers how to use all the functions on their machines but at the end of the day it is up to them to implement.

[Matthew Hajicek - Singularity]

I use it... CAMplete puts out G41.2/G42.2 when I use wear comp on 5-Axis toolpaths. :

 

FWIW, the new awesome 5-Axis toolpaths REMOVED CUTTER COMP  therefore I do not use them.

 

Yet another reason to stick with X9.

[Guest]

Yet another reason to stick with X9.

 

No, they were kind enough to leave the old 5-Axis toolpaths in there for us to use. :

 

I told CNC if they get rid of that I'm done with the product. Lacking that function would a deal breaker for me unfortunately. I do so much 5-Axis work, I HAVE to be able to output G41.2/G42.2. If it were not there, a key compeling reason to continue to use the product would be gone. We'll see how long it stays.

 

[Newbeeee™]

No, they were kind enough to leave the old 5-Axis toolpaths in there for us to use. :

 

I told CNC if they get rid of that I'm done with the product. Lacking that function would a deal breaker for me unfortunately. I do so much 5-Axis work, I HAVE to be able to output G41.2/G42.2. If it were not there, a key compeling reason to continue to use the product would be gone. We'll see how long it stays.

 

I really don't understand the reasoning why it would even be considered to remove it.

[Guest]

Prolly a Module Works issue/decision.