ALL TIPS FOR SWARF

[LucasGC]

Hi all,

Anyone know how to do this with multi passes? The linking page 

[crazy^millman]

Can you post up a screen shot with a little more detail?

[Guest]

Don't take any wooden nickels???

 

Those kind of tips 

[huskermcdoogle]

Depends on what you need to do...

 

[LucasGC]

Hi. sorry, that post was not about my problem I accidentally posted it. 

But grr, i do anger toward swarf. lol.

I've just kind of been playing with settings without knowing what they do, but I feel like with as much as I've messed around with them, I am still not closer to getting a smooth cut.

I switched to 3d curve with a chain as the guide and it works pretty well, feel like I could get it closer than I could with the swarf.

I don't know if this is a machine problem because it looks pretty smooth in mastercam in backplot, but when I run it it's got some pretty big steps that I can't see in mcam. 

I'm trying to make this with as much code as I can, thinking it will make it run smoother on a thermwood router. 

So this is what I've done:

Created untrimmed surface, offset the top rail 2 inches above bottom rail instead of only being .25 above. tried converting rails into lines/arcs, didn't see a difference, went back to 'curved edges' with 1 degree break tol. Have played with max step and tolerance values. tried tolerance at .01,.001,.0001 with max step at .001. I think it performed best at .01, but had one bigger step in it, .001 did fine and i'm thinking is what I will use if I can figure out how else to smooth it, .0001 was too slow and still jerky.

I prefer the cut strategy to sync with main axis, keeps it straight better.

Honestly I feel like there's so many settings that could be changed that I'm not going to find the 'one' that is wrong. 

I heard that thermwood machines like a ton of code, so I'm trying to make a toolpath with only line geometry 

bunch of questions/things I think I might have correct:

my max angle step is 1, and I have minimize rotation checked, why would you not check this?

none of my 'adjust feedrate' boxes are checked in utility tab - if I have points at a set distance then feedrate should be pretty consistent, yes?

in the misc tab there is a box for max angle step for rotation axis that I don't have checked. Recommended?

 

BASE.mcam

[huskermcdoogle]

Extend your vector out in backplot to the length of the first rotation pivot distance.  This is a good starting place to tell you how "kinematically smooth" the cut is for a head head machine.  It's pretty rough when you get out there with your path.

Looking into it, its due to your geometry.  The splines that create your upper and lower curves of the original surface have too much data and therefore at "noisy".   I took those edge curves from original surface, refit them with a .001" tolerance, then lofted a new surface and selected the new geo.  Then I set the tolerance to .0001, and turned off the .02 max step.  You now have a dense path without wavyness.

https://www.dropbox.com/s/342sdahueydugh8/BASE_Husker.mcam?dl=0

[huskermcdoogle]

Sometimes you need to fudge things a bit to get good results.  As long as at the end of the day you don't lose any overall accuracy (say in the case of optics machining), and can refit things within the cut tolerance you were expecting, it's the least painful route to accomplish what you are looking for.

[huskermcdoogle]

Lucas asked a few more questions via PM, I'll explain further here for the benefit of others in the future.

How did you know the splines were "noisy"?

-Create edge curve then check to see how many nodes they have.  If it is a simply shaped spline such as you had, you should likely have less than 20. I ended up with 32, but likely could have taken it further without much tolerance loss.  The original edge curves have 359 node points.

 

How do you extend the vectors in backplot (classic backplot) ?

-Go in the backplot options  (exclamation point in backplot control menu)

-Look under 4-5 Axis Tool Vectors and turn on the display, check connect top, and then length, and then put a value in, 6 to 10 inches is probably a good starting point.

 

[LucasGC]

Awesome, appreciate it. 

Also, I wasn't able to open your file, 'sim not enabled for necessary product'.

But I'm on to an even simpler part, have recreated the surfaces and curves, still jittery on the swarf toolpath though.

Tried decreasing my feedrate, that helped a little but i feel like this shouldn't be what i need to do - the machine should be able to cut as fast as the tool can handle, yes?

 

1.mcam

[huskermcdoogle]

SIm not enabled shouldn't be an issue.  Open the file and then drag the toolpath in the greyed out machine config into your machine config and you should be able to play with it.

[huskermcdoogle]

Depending, you may not be able to go all that fast.  All depends on how fast the machine needs to go at the control point (3 axis speed of the bridge, not tool tip)

[crazy^millman]

57 minutes ago, LucasGC said:

Awesome, appreciate it. 

Also, I wasn't able to open your file, 'sim not enabled for necessary product'.

But I'm on to an even simpler part, have recreated the surfaces and curves, still jittery on the swarf toolpath though.

Tried decreasing my feedrate, that helped a little but i feel like this shouldn't be what i need to do - the machine should be able to cut as fast as the tool can handle, yes?

 

1.mcam

No that is a router not a full on milling machine. Speeds and feeds need to be adjusted for cutting conditions 1st rule of any machining is not to think because the tool can handle the cut the machine can. Thermwood's are good routers, but they are just that a router and I can knock the head of a Thermwood router just sneezing on it (Not serious), but my point is I have cut some 5 Axis cuts at 800 ipm on a JOBS with a 840D and not think twice about it, but would never think to do the same thing on a Thermwood. I did some really trick stuff on the Thermwood's 15+ years ago, but it is all relative and think you need to manage your expectations. What is the speed and feeds you are trying to cut at? Might try filtering or might go to the extreme and give it 10X the code. See what is the right sweet spot and make that your go to process.

I have to say I do miss one machine I can sit an make programs for day in and day out from time to time. I have programmed well over a 100 different machine in the last 2 years and get a machine figured out and on to the next one get that one figured out and on to the next one. Once you have your process dialed in you need to make a tool library and ops library all dialed in. Then your programming will be just pretty much point and click and you will get bored real quick. Now I remember why I am doing what I am doing since that would get boring real quick.

[huskermcdoogle]

What is your C axis doing in these cuts, that is likely the limiting factor here.  If you were to tip the part such that the baxis stays positive or negative the entire time it will likely go much faster.

[LucasGC]

3 hours ago, C^Millman said:

No that is a router not a full on milling machine. Speeds and feeds need to be adjusted for cutting conditions 1st rule of any machining is not to think because the tool can handle the cut the machine can. Thermwood's are good routers, but they are just that a router and I can knock the head of a Thermwood router just sneezing on it (Not serious), but my point is I have cut some 5 Axis cuts at 800 ipm on a JOBS with a 840D and not think twice about it, but would never think to do the same thing on a Thermwood. I did some really trick stuff on the Thermwood's 15+ years ago, but it is all relative and think you need to manage your expectations. What is the speed and feeds you are trying to cut at? Might try filtering or might go to the extreme and give it 10X the code. See what is the right sweet spot and make that your go to process.

I have to say I do miss one machine I can sit an make programs for day in and day out from time to time. I have programmed well over a 100 different machine in the last 2 years and get a machine figured out and on to the next one get that one figured out and on to the next one. Once you have your process dialed in you need to make a tool library and ops library all dialed in. Then your programming will be just pretty much point and click and you will get bored real quick. Now I remember why I am doing what I am doing since that would get boring real quick.

 

I'm excited to get to point and click programming... just so satisfying to see a perfect part. I wasn't trying to run too fast, 300ipm. Now I've bumped it down to 100ipm, and it is a better.

What's your favorite way to recreate surfaces? I have one surface that has a lot of boundary points, i've tried curving the edges, refitting, untrimming original surface, and trimming back down to refitted splines, but still similar amount of boundary points. Then I used create flowline to create two u lines and two v lines, made a net surface from those, extended (was just a little off original surface) and then trimmed to boundary, still had similar boundary points.

Tip from thermwood was to set tol to .0005 for true 5-ax ops and .06" for max angle change. Haven't found the difference between max angle change in tool axis control tab vs misc tab.

3 hours ago, huskermcdoogle said:

What is your C axis doing in these cuts, that is likely the limiting factor here.  If you were to tip the part such that the baxis stays positive or negative the entire time it will likely go much faster.

it does retract, is that what you mean?

[huskermcdoogle]

3 minutes ago, LucasGC said:

it does retract, is that what you mean?

More so is your C axis moving 360 degress to perform the cut?  If you tip the part so the B axis stays away one side of positive or negative, you won't need 360 degrees of C travel.  you might only need 20 or so.  This will greatly reduce the amount of movement the machine needs to do, thus it should be smoother and faster.

[LucasGC]

 

18 minutes ago, huskermcdoogle said:

More so is your C axis moving 360 degress to perform the cut?  If you tip the part so the B axis stays away one side of positive or negative, you won't need 360 degrees of C travel.  you might only need 20 or so.  This will greatly reduce the amount of movement the machine needs to do, thus it should be smoother and faster.

Okay, yes i think i could tilt it, i don't mind the retract, i would rather figure it out this way than tilting all the parts I need to run swarf on :/

Running the swarf with .06" angle inc seems a little worse, ha. But I do see the wavy vectors in backplot, so It should just be something I need to tweak. Posting a pic of the vectors, seems decent to me, definitely wavy, but smooth wavy. Not sure what else to do with my geometry to get a smoother path.

TOP.mcam

[LucasGC]

lol running with auto control strat:

[huskermcdoogle]

What you are dealing with is the fact that the splines don't have the same number of node points.

[LucasGC]

Oh, I thought I was just worried about them having too many. How would I get them to have the same number of points if they are different curves though? I mean wouldn't different geometry need different points?

This is also a problem for me when I try lofting surfaces, and I don't have splines with the same start point, the surface gets all twisty.

[huskermcdoogle]

All of the things that you just mentioned are issues that I just don't have good answers for.   You can make the splines have the same start point by breaking them by the same line from a common view, and then creating a new spline from the remaining curves.  Chain the spline from the new start location you are looking for.

One thing to note, if you extend the surface, you have the same waviness present.  You get a good clean surface, you will have a good clean cut.  How to get there? Well not sure I can help, but maybe someone else can chime in and give us an aha moment.

[LucasGC]

2 minutes ago, huskermcdoogle said:

All of the things that you just mentioned are issues that I just don't have good answers for.   You can make the splines have the same start point by breaking them by the same line from a common view, and then creating a new spline from the remaining curves.  Chain the spline from the new start location you are looking for.

One thing to note, if you extend the surface, you have the same waviness present.  You get a good clean surface, you will have a good clean cut.  How to get there? Well not sure I can help, but maybe someone else can chime in and give us an aha moment.

Dang, yeah I did notice the surface is wavy if it's extended :/ Have tried a bunch of lines types but I will keep trying! Wondering why it's wavy in the first place. Just not created well or conflicts between programs?

[huskermcdoogle]

All goes back to the base geometry.  If you know how it was modeled, or what the design intent was, you could probably fix it without much trouble.

[huskermcdoogle]

If it is just draft from veritcal (which it appears to be), Curve 5 Axis, -3 degrees side tilt angle, use top plane for tool axis control, chain the bottom curve, .25 radial offset.  Then play with the tolerance and whatnot for you step along to get rid of faceting.

[huskermcdoogle]

Try opening this and see what I did.

https://www.dropbox.com/s/7tr7tw9d26uv3pk/TOP_Husker.mcam?dl=0

[LucasGC]

23 hours ago, C^Millman said:

No that is a router not a full on milling machine. Speeds and feeds need to be adjusted for cutting conditions 1st rule of any machining is not to think because the tool can handle the cut the machine can. 

I guess I was giving the machine an unrealistic feedrate, and then thinking the tolerance would just keep it at the max feedrate it could handle. Can the machine calculate feedrate based on look ahead or is it per line segment?