Surface Quality

[LucasGC]

Hello

I'm having trouble finding which settings to change to control the surface finish of the part after it's machined.

I've lowered the tolerance from .025 mm to .01 mm and that helped, but I think there should be something else I can change to create a smooth toolpath rather than a jerky one that doesn't x100 the file size. Mostly it's just a little wobbly, when it's in 3-axis it leaves a pretty nice finish. When it switches to 5-ax however some movements are very rapid and have heavy jitters. We have a beast of a machine so rigidity and structure shouldn't be a problem.

I'll upload the part to show what I'm working with, if anyone has recommendations on how to make a faster, smoother toolpath all help is appreciated. 

standoff mold rh.mcam

[huskermcdoogle]

Couple of quick questions:

Which toolpath in the file are you wanting to improve? The Swarf path?

What machine and control do you have? 

What do you have for high speed options?  These options could mean an easy button for a smooth path.

Otherwise, there isn't much you can do to keep the file size down, as your goal is going to be to lower the linear and rotary acceleration between block points.  To do this, you can either lower your max angle tolerance, or your chordal error.  Sometimes if the issue is just rotary acceleration, you can create a smoother pattern surface and use that to drive your tool axis.

In the case of the swarf path, there are many different ways to "optimize" the path.  I have found it usually helps to create upper and lower curves, sometimes you even need to create upper curves that are much higher than on the part.  This gives the algorithm more to work with so to speak, and you won't get as much along cut direction tipping.  Sometimes using tilt lines helps, but I have found it doesn't get as nice of results on a lot of circuitous applications.

Anyway, I would gladly play with what you have, but I can't as I don't have a seat of router...

[LucasGC]

Hello, if any of them could be improved I would like to know how, but yes the swarf is currently the only one that is jittering enough to gouge the part past the point of being able to sand smooth.

We have a thermwood model 70 with thermwood control, and should have all the high speed options available, though I don't know specifically what you're referring to. 

I will try changing the max angle tolerance, that's something I haven't messed with yet.

And yes, the swarf is tricky, I wish there was an option to keep the tilt as flat to the floor surface as possible

[CEMENTHEAD]

Use G93 Inverse Time

"When combined linear/rotary motion exists. Each combined linear/rotary move has a different distance. Thus the corresponding time values change for each code block, even if it does not change from the previously programmed feed value. Invoking Inverse-Time Mode

A G93 is necessary to declare the feed mode on the initial move containing rotary motion.

General Rule: If a G93 is necessary to invoke inverse time mode, a G94 is necessary to cancel it.

This means that the first move of a sequence of normal XYZ linear moves with no rotary A/B/C words must have a G94 and an F that is interpreted in inches per minute.

G93 lets the user follow a more complex tool path when linear/rotary axes are involved. lets the user have better control of the rotary's motion. This gives a more precise part with a better surface finish."

this was Copy n pasted from notes.

Edited May 4, 2018 by CEMENTHEAD
its friday...

[huskermcdoogle]

Don't know anything about the thermwood control.  In fanuc land, AICC, High Speed Tool Posture Control, and Nana Smoothing 2 would be the options that would allow you to cook with gas, without having to do a ton of work on the CAM side of things.

[crazy^millman]

The Thermwood has a tangency control factor. Also feed it tons of code make your angle and step overs small and and you will get better surface finish. I use to make molds out of Renshape 5’ x 10’ and they almost never had to be touched after machining. Yes they would run for up to 170 hours, but when it was done and ready to mold a part off the machine untouched it was a good feeling. 

[LucasGC]

@CEMENTHEAD Thank you, I have seen these options and have not experimented with them. Does TCP change the g93? My default is g96 but the tcp turns it into a g95. I tried just changing the code from g96 to g93 and did not notice a difference. I'm curious which notes you mean and who they're available to.

@C^Millman Thanks, I've played with the tangency factor and have my default set to 10. I'm nervous about going all the way to 40 because I feel like it would be pretty far off from the part, and if it isn't, why wouldn't that be what everyone uses?

 

I guess I'm just figuring it all out still. Like today, realized that the hi-speed toolpaths take a really long time with almost non-existent step-overs where a parallel spiral slows down at the corners but flies through everything else (even though it leaves stock in some places, I'll have to try the constant overlap spiral next).

I had a particularly bad Swarf mill toolpath today. I played with it a bit and found that running at a .001mm tolerance at least slowed it down enough to keep it on the wall I was trying to cut. However, it also slowed it down significantly around a big smooth curve. I had the fanning and max angle step set to 1 (are these the same thing) and the minimize rotation axis changes checked - as well as the adjust feedrate on edges and for fanning checked.

One thing I plan on doing for my next part is importing the solid file, converting it to surfaces, and only working with that to create the geometry/toolpaths. Will this provide me with a cleaner surface to generate a smoother toolpath?

Thanks

[huskermcdoogle]

56 minutes ago, LucasGC said:

Will this provide me with a cleaner surface to generate a smoother toolpath?

Maybe but not likely.

[LucasGC]

On 5/5/2018 at 10:33 AM, C^Millman said:

The Thermwood has a tangency control factor. Also feed it tons of code make your angle and step overs small and and you will get better surface finish. I use to make molds out of Renshape 5’ x 10’ and they almost never had to be touched after machining. Yes they would run for up to 170 hours, but when it was done and ready to mold a part off the machine untouched it was a good feeling. 

So at this point I've got my toolpaths pretty minimalized, very few points. However my machine is still slowing down at each of these points, it's like the tangency factor isn't working. 

Would someone like to look at this part and give me some ideas for optimizing? 

Again, I'm happy with the points along my toolpath, just looking to speed it up. 

Changing feedrate doesn't seem to help, might be an acceleration problem but I have it set to default G800.

Specifically, on the 3d curve toolpath it almost stops at every point, and the lead in/lead out curve is broken into lines as well, is there a way to break it into one smooth curve with two points?

Any help is appreciated.
Thanks

GB1-5314-10-02 Lower.mcam

GB1-5314-10-02 Lower.nc

GB1-5314-10-02 Lower T4.nc

[crazy^millman]

34 minutes ago, LucasGC said:

So at this point I've got my toolpaths pretty minimalized, very few points. However my machine is still slowing down at each of these points, it's like the tangency factor isn't working. 

Would someone like to look at this part and give me some ideas for optimizing? 

Again, I'm happy with the points along my toolpath, just looking to speed it up. 

Changing feedrate doesn't seem to help, might be an acceleration problem but I have it set to default G800.

Specifically, on the 3d curve toolpath it almost stops at every point, and the lead in/lead out curve is broken into lines as well, is there a way to break it into one smooth curve with two points?

Any help is appreciated.
Thanks

GB1-5314-10-02 Lower.mcam

GB1-5314-10-02 Lower.nc

GB1-5314-10-02 Lower T4.nc

Any reason why you want to one way the features and not zig zag them? Can you go 90 to the direction you have chosen and get nicer motion? Been many years since I programmed a Thermwood, but would think you could get a hold of their AE staff and they could give you some pointers to help make this go in the direction you need. 

[LucasGC]

53 minutes ago, C^Millman said:

Any reason why you want to one way the features and not zig zag them? Can you go 90 to the direction you have chosen and get nicer motion? Been many years since I programmed a Thermwood, but would think you could get a hold of their AE staff and they could give you some pointers to help make this go in the direction you need. 

I'm going one way at the angle I am going because the material I am cutting is aramid honeycomb. I don't want to zig-zag because a big stepover while in the material could stretch/distort it. I am machining at the angle I am because it pushes the material down toward the vacuum board, which is nice because the only thing holding the honeycomb is a piece of paper vacuumed to the top. Contacted Thermwood and sent a file, just thought I would get input from two sources and try everything.

[crazy^millman]

1 hour ago, LucasGC said:

I'm going one way at the angle I am going because the material I am cutting is aramid honeycomb. I don't want to zig-zag because a big stepover while in the material could stretch/distort it. I am machining at the angle I am because it pushes the material down toward the vacuum board, which is nice because the only thing holding the honeycomb is a piece of paper vacuumed to the top. Contacted Thermwood and sent a file, just thought I would get input from two sources and try everything.

Okay that makes perfect sense and I understand exactly why you must do it the way you are doing it. Nothing stands out at me expect playing with settings on the tangency factors and see if any of them give you better results. Your toolpaths look correct and the way you are cutting should be pretty cut and dry and move with no issues. I cut more complex stuff that this 15 year ago on Thermwood's and it always did a great job for me.

[Müřlıń®]

 

I have zero experience on that control.

 

But I did an internet search and found a possible fix.

Use G93 and set control to "constant velocity" instead of "constant stop".

 

[LucasGC]

I've tried all the feed rate modes - g93-96 - with no luck

I have my acceleration set to default G800

And my tangency is now back to default 1 - playing with this I found that no matter the value it always stops at the points, but with a higher value it slows down further before it reaches the point.

 

IMG_0561.3gp

[LucasGC]

On 6/4/2018 at 2:53 PM, C^Millman said:

Okay that makes perfect sense and I understand exactly why you must do it the way you are doing it. Nothing stands out at me expect playing with settings on the tangency factors and see if any of them give you better results. Your toolpaths look correct and the way you are cutting should be pretty cut and dry and move with no issues. I cut more complex stuff that this 15 year ago on Thermwood's and it always did a great job for me.

Man I'm still having problems getting this thing to move smoothly...

Was using the parallel stepover toolpath for pocket cuts because the high speed creates more complex toolpaths and generates slower motions, thought I had figured out the filtering a little better so I went back to try the high speed again. Same problem except now I know my toolpaths are smooth the machine just isn't having it.

agnuagiagasernjernqrjnq

 

IMG_0568.3gp

[LucasGC]

that last post has a video file too as a demonstration for how SLOW it is

I'm cutting foam, i need this thing flying through it

fnasdgnfasganga

[crazy^millman]

Give it more code and need to set the look ahead. I use to feed our Thermwoods at 1200 imp all day long with no issues. I use to do full 5 Axis moves and everything again with no issues at 300 and 400 ipm. There has to be something going on with the control. Again what does Thermwood have for an answer? I would be on the phone with them every 5 minutes until someone gave me a good answer.

[huskermcdoogle]

I concur with Ron, you got something funky going on.  Do you have any programs that run right?

[Müřlıń®]

The internet said there is a setting to choose between constant step or constant velocity...has to be set at the control.

[LucasGC]

I've been emailing, nothing about the control yet. 

They sent me back a cimco edit picture of my toolpath after it posts, and the curves are very jagged.

First of all upset I don't have cimco

Second how the heck 

what

[huskermcdoogle]

I would look into changing the chord_tol$ (tolerance for linarc$) in the post.  I have not seen there be a custom value for chord_tol$ not sure where that is set.  Maybe Colin can chime in.

[LucasGC]

Yeah, so is it possible that I have a smooth 3d arc in mcam and then my post breaks it down into non-smooth lines?

[crazy^millman]

2 hours ago, LucasGC said:

Yeah, so is it possible that I have a smooth 3d arc in mcam and then my post breaks it down into non-smooth lines?

Yes it is where you need to go back to your post builder and ask them how they handle those situations. Could be in the CMD also.

[huskermcdoogle]

I had some time to kill for a bit this morning so I looked things up.

Look into making the tolerance tighter on the following.

 

 

 

That should be what sets chord_tol$.

[LucasGC]

Husker thanks so much, how did you go about finding this?

I feel like i have googled every question to this and have not found an answer like changing chordal deviation.

Unfortunately, it didn't help. I changed it from .02 to .00127, which was the default on the post.

My tolerance page does look slightly different, and my curve chordal dev does not say 'used in post' like yours does, but i'm sure it still is.

Next i will go through my post and see if i can set any of the other tolerances in mcam to the post tolerance value. 

 

 

Just got another email saying 'every customer experiences this and has to learn what settings work best'

Is this not a matter of setting the tolerance in mcam to be the same as the tolerance in the post??

Do i absolutely need cimco edit do guarantee that my toolpaths will run smoothly?