Swarf Machining stuttering on C-axis

[Metallic]

Hey all,

I'm having this issue with stutter on my C-axis rotary when I run this swarf toolpath. Angular step is 3deg and Cut Tolerance is 0.0005, if I set that to 0.001 or 2 the stuttering is less but the surface sucks. I've never had this with Swarf ever. Also it isn't a particularly complex toolpath.

Any ideas about how to get a smooth finish using swarf? I try to bump the surface finish parameter up in Misc Reals as well to no good result. The wall is tapered at 88.9 degrees.

[#Rekd™]

Can you drive it with curves instead?

[Metallic]

37 minutes ago, #Rekd™ said:

Can you drive it with curves instead?

I suppose im not 100% sure what you mean. In the swarf machining toolpath there need to be drive surfaces, and I have an upper and lower rail that I am using for guide curves.

I was contemplating if there is a  way to use vector lines to maintain the tilt or something. I'm going to upload the solid part, maybe im missing something. I can't upload my .EMCAM file because it is too big.

INLET_RING.SLDPRT

 

Also, I dunno if this is possible but to output as a 4 axis toolpath so the A axis tilts but the move is carried out only by XandY. The inner walls arent tapered, only the arc

[Guest]

13 minutes ago, Metallic said:

I suppose im not 100% sure what you mean. In the swarf machining toolpath there need to be drive surfaces, and I have an upper and lower rail that I am using for guide curves.

I was contemplating if there is a  way to use vector lines to maintain the tilt or something. I'm going to upload the solid part, maybe im missing something. I can't upload my .EMCAM file because it is too big.

INLET_RING.SLDPRT

 

You can use only curves

[crazy^millman]

Sorry I missed this was a 4 axis machine. None of this is usable on a 4 Axis machine. You will have to 3D surface machine that taper on that machine.

I would model prep it and then drive it from the walls and call it a day.

Here is the file programmed and set to run what I think should be good on your machine. Sorry I used a BACK WCS to Program it to.

5TH AXIS INLET RING

Also with Model prep give you an easy way to make the upper and lower chains directly from a solid to drive the toolpath that way if you so choose.

I added conservative feed 2d Dynamic Roughing from the Model Pep Solid. The line is to help the stupid non aware of the Tool Plane Linking in 2021. I believe 2022 finally respected the Tool plane in the Linking Parameters.

[Metallic]

1 hour ago, crazy^millman said:

Sorry I missed this was a 4 axis machine. None of this is usable on a 4 Axis machine. You will have to 3D surface machine that taper on that machine.

I would model prep it and then drive it from the walls and call it a day.

Here is the file programmed and set to run what I think should be good on your machine. Sorry I used a BACK WCS to Program it to.

5TH AXIS INLET RING

Also with Model prep give you an easy way to make the upper and lower chains directly from a solid to drive the toolpath that way if you so choose.

I added conservative feed 2d Dynamic Roughing from the Model Pep Solid. The line is to help the stupid non aware of the Tool Plane Linking in 2021. I believe 2022 finally respected the Tool plane in the Linking Parameters.

Sorry I didnt mean to confuse anyone Ron, I am running this on a  5 axis trunnion machine....I was asking if I could output it as a 4 axis output on a 5 axis machine. Do you have a EMCAM file I could bum?

1 hour ago, Thee Byte™ said:

 

You can use only curves

I am using the Swarf Machining toolpath from Moduleworks

[Guest]

2 minutes ago, Metallic said:

Sorry I didnt mean to confuse anyone Ron, I am running this on a  5 axis trunnion machine....I was asking if I could output it as a 4 axis output on a 5 axis machine. Do you have a EMCAM file I could bum?

I am using the Swarf Machining toolpath from Moduleworks

Yes, if you use the other one it doesn't need surface(s)

[crazy^millman]

29 minutes ago, Metallic said:

Sorry I didnt mean to confuse anyone Ron, I am running this on a  5 axis trunnion machine....I was asking if I could output it as a 4 axis output on a 5 axis machine. Do you have a EMCAM file I could bum?

 

You cannot do that in a 4 Axis only process. That must be cut in a full 5 axis toolpath to make it come out correctly. Sorry I don't have a emcam file, but I thought you could open regular Mastercam files in them. If not try importing the operations.

[Metallic]

16 minutes ago, crazy^millman said:

You cannot do that in a 4 Axis only process. That must be cut in a full 5 axis toolpath to make it come out correctly. Sorry I don't have a emcam file, but I thought you could open regular Mastercam files in them. If not try importing the operations.

Yes Ron youre correct you can open mcam files with edu license. Thank you for the help, I will take a look at that toolpath to see how it runs/

[crazy^millman]

10 minutes ago, Metallic said:

Yes Ron you're correct you can open mcam files with edu license. Thank you for the help, I will take a look at that toolpath to see how it runs/

The work here was using Model prep to make a good solid edge to drive the swarf from. What you had can be done, but the more normal the wall like i did the better swarf seems to work. When Swarf has to take full walls and half walls and do the toolpath things get wonky. Where Peter was correct in saying drive it by chains, but as a long time wireframe user for 5 Axis I am doing less and less wireframe for 5 axis toolpaths. In general for most toolpaths. Solids as a process have come a very long way in Mastercam. Why I made the model I did to start showing people how much it has progressed. Mike at CamInstructor just happen to catch me at a good time to turn what I was going to do on the forum into Ron Week for them. Funny thing is none of that was scripted or planned. He caught me at the right time and place to do what we did. I try not to be too hard on myself, but I think it was a train wreck to be honest. Mike said it was well received and many people have thanked me for doing it so I say okay glad for it. 

[Guest]

It makes sense, since you are dealing with very large files, the wireframe is only going to make the file larger.

Wireframe is very flexible, however Ron is correct, the solids in Mastercam are improving..

[motor-vater]

singularity issue maybe???

 

[Metallic]

1 hour ago, crazy^millman said:

The work here was using Model prep to make a good solid edge to drive the swarf from. What you had can be done, but the more normal the wall like i did the better swarf seems to work. When Swarf has to take full walls and half walls and do the toolpath things get wonky. Where Peter was correct in saying drive it by chains, but as a long time wireframe user for 5 Axis I am doing less and less wireframe for 5 axis toolpaths. In general for most toolpaths. Solids as a process have come a very long way in Mastercam. Why I made the model I did to start showing people how much it has progressed. Mike at CamInstructor just happen to catch me at a good time to turn what I was going to do on the forum into Ron Week for them. Funny thing is none of that was scripted or planned. He caught me at the right time and place to do what we did. I try not to be too hard on myself, but I think it was a train wreck to be honest. Mike said it was well received and many people have thanked me for doing it so I say okay glad for it. 

Always you are a big help to the community, the model prep setup step alone has helped a ton! Most of the time I am using straight solids for driving my toolpaths, but multiaxis sometimes I need surfaces and lots of random wireframe. I started on X7 and would say solids have improved a ton since then for sure.

[Leon82]

Check the box that says minimize rotation changes. And change the maximum step to a very low amount

[cncappsjames]

I typically run my cut tolerance between .0025" and .0005" and my point spacing between. 005" and .010". 

The tolerance is dictated by the print tolerances and the spacing is dictated by finish requirement.

On a quality machine, .010" spacing is pretty much indistinguishable from feed lines. 

HTH

[huskermcdoogle]

14 hours ago, cncappsjames said:

I typically run my cut tolerance between .0025" and .0005" and my point spacing between. 005" and .010". 

The tolerance is dictated by the print tolerances and the spacing is dictated by finish requirement.

On a quality machine, .010" spacing is pretty much indistinguishable from feed lines. 

For the un-initiated, this information is Gold.  It took me a long time to realize similar numbers was were things typically run best.  Sometime I will end up using a smaller tolerance, but that point spacing just runs good in most cases and isn't overwhelming to really any modern control data wise.  Also with the MW swarf toolpath.  .0008 vs .001 can make a world of difference in the actual toolpath result depending on the input geometry quality.  I sometimes have to sit here and tweak the tolerance by .0001 or so at a time and end up with completely different toolpaths.  A .0001 difference can be the difference between a super smooth swarf path or a total abortion that you won't even be willing to run in verify....

[Zaffin_D]

On 3/19/2021 at 5:57 PM, motor-vater said:

singularity issue maybe???

 

I'd expect the motion on the inside corners to be erratic.  Start at the lower right of the below image; notice how the flags (dark purple) are nicely flowing?  Once we hit the corner, big swings start to happen.

 

This could be avoided by fixturing the part at an angle, or by smoothing the instability across multiple moves.  The result of the latter is shown below.

 

[So not a Guru]

On 3/19/2021 at 11:22 PM, cncappsjames said:

I typically run my cut tolerance between .0025" and .0005" and my point spacing between. 005" and .010". 

The tolerance is dictated by the print tolerances and the spacing is dictated by finish requirement.

On a quality machine, .010" spacing is pretty much indistinguishable from feed lines. 

HTH

 

On 3/20/2021 at 1:59 PM, huskermcdoogle said:

For the un-initiated, this information is Gold.  It took me a long time to realize similar numbers was were things typically run best.  Sometime I will end up using a smaller tolerance, but that point spacing just runs good in most cases and isn't overwhelming to really any modern control data wise.  Also with the MW swarf toolpath.  .0008 vs .001 can make a world of difference in the actual toolpath result depending on the input geometry quality.  I sometimes have to sit here and tweak the tolerance by .0001 or so at a time and end up with completely different toolpaths.  A .0001 difference can be the difference between a super smooth swarf path or a total abortion that you won't even be willing to run in verify....

@cncappsjames & @huskermcdoogle, I get that the point spacing, on Swarf, is the max distance on the Cut Pattern page.

But when using 5X Curve, there are three different fields that confuse me; On the Cut Pattern page there are two sections; Curve type, that has "distance increment" & Curve following method, that has the choice between "Distance" or Maximum step"

How do you use these to get smooth movement?

[huskermcdoogle]

6 hours ago, So not a Guru said:

How do you use these to get smooth movement?

It's been so long I don't honestly remember.  But what I do remember is when using 5x Curve.  Filter setting, and tool axis control have more importance on the smoothness of the path than the curve following method itself.  Of course the curve following method will influence the "resolution" of the tool axis control and overall motion of the machine, but the "smoothness" of the tool axis control is more dictated by the method of which you pick. 

Way too many ways to skin the cat once you get into 5x Curve to take a guess on what you should/could be doing....  Post up or send me an example of what you are trying to do, and I will see what I can do to make it "smooth".  I'm sure Ron or James would love to pitch in as well.  More generic the better as all can learn if we make it public.

When I think of making a smooth 5x toolpath, my brain immediately starts thinking in terms of physics and calculus.  Determine the outcome desired, then balance that with the cutting velocity required, then you can think in terms of acceleration in XYZ, and then in the case of acceleration of the rotary axes, which IMHO will slow things down more than accel/decel issues in straight XYZ, as they affect the XYZ motion directly NO MATTER WHAT, further from center ->> the worse it gets.   This is where options like the smooth TCP / posture control function on a Fanuc control actually smooth out the angular displacement issues between points which cause great acceleration changes in the rotary and translational axes.  If you don't have those options, you have to do that at the toolpath level, which can be done with time, patience, and knowing how to recognize and eliminate the trouble spots.  This is typically the way to get the absolutely fastest path anyway, so for long run stuff you may as well start to develop your process on doing it.   

Food for thought: if you have a generic non-tcp post, posted from centerline(s) of rotation, you can edit the post to actually calculate and output acceleration values for each axis at each point and you can theoretically use that code to look for your hot spots mathematically, and then subsequently know where you will have areas on the machine that will greatly slow it down.  I haven't done it yet, but I think there is a function on the post side of things that you can use to draw geometry on a level in mastercam.  You could in theory use that to draw a visual representation of the toolpath that met certain criterial for acceleration, so you could visually pinpoint the trouble spots.  Many times it is just a matter of tweaking a few vectors, or deleting a point here and there.  I have written filters in excel that filter the NCI, I then import NCI and post the paths.  Sometimes resulting in 50% or greater reduction in cycle time, with vastly improved surface finish due to constant cutting velocity.

blabber blabber blabber, I could go on forever.  I'll stop now, before I dig a big hole where I need to explain myself. 

[gcode]

One thing I've found working with 5X toolpaths

If you have MachineSim, use it.

I have a home made machine sim for our Okuma MU.

It does a very good job of showing stuttering bouncy 5X toolpaths.

In fact it does a better job of showing toolpath instability than Vericut does.

If machine sim shows a toolpath is performing poorly, it will perform poorly on the machine

even if backplot and Vericut run smoothly.

[Guest]

46 minutes ago, gcode said:

One thing I've found working with 5X toolpaths

If you have MachineSim, use it.

I have a home made machine sim for our Okuma MU.

It does a very good job of showing stuttering bouncy 5X toolpaths.

In fact it does a better job of showing toolpath instability than Vericut does.

If that machine sim shows a toolpath is performing poorly, it will perform poorly on the machine

even if backplot and Vericut run smoothly.

I built my first machine Sim for a 5 axis router today, it was surprisingly easy, the machine simulation is great.. Wish I had vericut of course..

[Metallic]

Hmmm interesting…I’ve generally avoided MachSim since I tried to put my machine in there and it didn’t work so I gave up. I run vericut now tho. 
 

so say I have all the machine models from our MTB…any good resources on how to get everything into machsim properly? I think I remember that things need to be in XML format?

 

thanks 

On 6/1/2021 at 12:53 PM, gcode said:

One thing I've found working with 5X toolpaths

If you have MachineSim, use it.

I have a home made machine sim for our Okuma MU.

It does a very good job of showing stuttering bouncy 5X toolpaths.

In fact it does a better job of showing toolpath instability than Vericut does.

If machine sim shows a toolpath is performing poorly, it will perform poorly on the machine

even if backplot and Vericut run smoothly.

 

[Colin Gilchrist]

44 minutes ago, Metallic said:

Hmmm interesting…I’ve generally avoided MachSim since I tried to put my machine in there and it didn’t work so I gave up. I run vericut now tho. 
 

so say I have all the machine models from our MTB…any good resources on how to get everything into machsim properly? I think I remember that things need to be in XML format?

 

thanks 

 

Models need to be STL format. The XML file is used on the machine simulation definition, where you edit/define the kinematic tree.

[Guest]

6 hours ago, Metallic said:

Hmmm interesting…I’ve generally avoided MachSim since I tried to put my machine in there and it didn’t work so I gave up. I run vericut now tho. 
 

so say I have all the machine models from our MTB…any good resources on how to get everything into machsim properly? I think I remember that things need to be in XML format?

 

thanks 

 

Cam-Instructor has a few tutorials on building machines. @mwearne

Once you are inside the editor and adding stl files to the machine it goes fast, even for more complex machines.

If you can't get it working I can take a look. 

The xml tags are holding a reference to all the stl files in your machine, tool and workpiece groups,collision detectors etc.

 

[Metallic]

Thanks I will try this out when I get back into the shop. Would be nice to have both MachSim and Vericut.

 

Is it true that MachSim can now verify posted Gcode? I can't remember exactly where I recently saw a video that said you can simulate posted code within Mastercam.

EDIT: I believe it was some recent webinar..maybe ShopWare or someone else went through it