MasterCAM posting out all splines during surfacing radii

[TerraXJ]

Lately I've noticed that 2017 MasterCAMs surfacing is worse than it used to be. Posting wise atleast. Lots of splines being posted when they should be ARCs. I have been playing with all the settings, filters and trying different values but nothing seems to helps. Only thing I have noticed is being able to increase the size of the spline, making tool path very choppy. 

I have a very clean STEP file i'm working with so that can't be the problem, and i'm machining a simple taper. This should be generating a G03 just at different depths... right? 

Anyone been able to reduce the toolpath size and generate ARCs?

Its running on a Haas VF4 that has HSM enabled, so i don't think its the control thats the problem. Also I have run different G187 P3 E x.xx settings with out any difference in surface finish quality.

 

This is what my code is looking like.

(T6   - 0.5 SPHERICAL / BALL-NOSED ENDMILL - H6   - D6   - D0.5000" - R0.2500")
G00 G17 G20 G40 G80 G90
G91 G28 Z0.
(COMPENSATION TYPE - COMPUTER)
T6 M06 (0.5 SPHERICAL / BALL-NOSED ENDMILL)
(MAX - Z.25)
(MIN - Z-1.3371)
(TOOLPATH - FINISHFLOW)
(STOCK LEFT ON DRIVE SURFS = 0.)
G00 G17 G90 G54 X18.0025 Y-1.4534 S7000 M03
G43 H6 Z.25
M08
Z-1.2371
G94 G01 Z-1.3371 F60.
X18. Y-1.3034
X17.9913 Y-1.3036
X17.9711 Y-1.3051
X17.951 Y-1.3081
X17.9313 Y-1.3127
X17.912 Y-1.3189
X17.8932 Y-1.3265
X17.8751 Y-1.3356
X17.8578 Y-1.3461
X17.8414 Y-1.358
X17.8259 Y-1.371
X17.8115 Y-1.3853
X17.7982 Y-1.4006
X17.7862 Y-1.4169
X17.7756 Y-1.4342
X17.7663 Y-1.4522
X17.7584 Y-1.4708
X17.752 Y-1.4901
X17.7472 Y-1.5097
X17.7439 Y-1.5297
X17.7422 Y-1.5499
X17.7421 Y-1.5702
X17.7436 Y-1.5904
X17.7467 Y-1.6104
X17.7513 Y-1.6301
X17.7575 Y-1.6494
X17.7651 Y-1.6682
X17.7742 Y-1.6863
X17.7847 Y-1.7036
X17.7965 Y-1.7201
X17.8096 Y-1.7356
X17.8238 Y-1.75
X17.8392 Y-1.7632
X17.8555 Y-1.7752
X17.8727 Y-1.7859
X17.8907 Y-1.7952
X17.9094 Y-1.803...........

[mkd]

did you try check boxing "output 3d arcs?

[mkd]

you can do a contour for that with a draft angle.

[jlw™]

29 minutes ago, mkd said:

you can do a contour for that with a draft angle.

That's how I do these type of features.  No surface creation, containment or check... just one closed arc and BOOM.

 

One more time, BOOM!

[nickbe10]

If it were me I would have started with waterline......but mkd is also correct (and jlw_edit), many ways to skin the cat. One thing I learned early on with surfacing is if the first toolpath doesn't give you what you want quickly, ghost out the toolpath and try something else. I might do this 3 even 4 times before deciding which method to start tweeking into submission......

[jeff]

For giggles, get rid of your check surfaces and see how the code looks then.

 

[TerraXJ]

37 minutes ago, mkd said:

did you try check boxing "output 3d arcs?

Yes, doesn't change anything.

 

36 minutes ago, mkd said:

you can do a contour for that with a draft angle.

Problem with that is, it will only cut from top - down.

5 minutes ago, nickbe10 said:

If it were me I would have started with waterline......but mkd is also correct (and jlw_edit), many ways to skin the cat. One thing I learned early on with surfacing is if the first toolpath doesn't give you what you want quickly, ghost out the toolpath and try something else. I might do this 3 even 4 times before deciding which method to start tweeking into submission......

A Surface High Speed Waterline? I don't see a Waterline toolpath under my "Surface Finish" only under "Surface High Speed Toolpaths". Just tried it and that produced many spines too.

The point I was trying to get to is that this toolpath is super simple. So simple in fact you can pretty much manually do this code or doing a work around by a tapped contour as stated by "mkd" but why can't change direction of plunge? How hard would it be for them to of added check box for plunge direction?

Over time it seems that MasterCAM always requires many work around to achieve simplistic toolpaths. 

[Guest]

Turn off the smoothing(overkill) and tighten up the tolerance to .0005" set line/arc tolerance to 66.7%

If that doesn't get it. the geometry is not in a flat plane.  Isee the G94 and wonder if this is on some kind of tilt

 

I would like to see a file...this is a non-issue so I am curious a to how it is setup

Edited March 9, 2018 by Guest

[TerraXJ]

2 minutes ago, jeff said:

For giggles, get rid of your check surfaces and see how the code looks then.

 

I only used 1 drive surface.

[Guest]

Basic.....in 2017 file

flowline arcs.mcam

Edited March 9, 2018 by Guest

[Colin Gilchrist]

Turn off the "one way filtering", and do not use "Smoothing" if you want Arcs.

I'd make your total tolerance .002. And make your Cut Tolerance .0002 (10%), and your Line Arc Filter Tolerance .0018 (90%).

Inside the Arc Line Filter itself, set the option to "Tighten Line Filtering", and set that to 5-10%. (You are telling the Filter to Bias towards ARCS by using less tolerance for the "Line" portion of the Filter.)

[CEMENTHEAD]

If you want lines, that's how you get lines. 

 

(Depth cuts at angle will give you nice arcs)

[mkd]

2 hours ago, CEMENTHEAD said:

If you want lines, that's how you get lines. 

 

(Depth cuts at angle will give you nice arcs)

LOL. Um yeah, that'll give you lines. If it was a snake it would have bit me/

I never turn smooth settings on, so wasn't even think of that.

 

 

also, For that type of feature with flowline, i like to use spiral, not one way. 2 cents

[TerraXJ]

On 3/9/2018 at 10:59 AM, CEMENTHEAD said:

If you want lines, that's how you get lines. 

 

(Depth cuts at angle will give you nice arcs)

"Lana do you want lines, because thats how you get lines!" Ha ha fellow Archer fan I see.

Yeah of all the things i was playing with and trying I didn't see that option but I suspect that wouldn't have helped my situation. I turned off "Smoothing" and turned the "Line/Arc Tolerance" up to 60% and that was the fix. Nice clean Arcs now. This was a OE (operator error) 

So what is that "Smoothing" option even useful for?

Sorry for the delay in posting, I'm a noob so they limit my posts till i get my 10 post street cred.

[Guest]

I really only use the smoothing options on machines with G05 look-ahead that prefer line code instead of arcs....

 

Edited March 12, 2018 by Guest
if I could only spell :)

[Colin Gilchrist]

15 minutes ago, TerraXJ said:

"Lana do you want lines, because thats how you get lines!" Ha ha fellow Archer fan I see.

Yeah of all the things i was playing with and trying I didn't see that option but I suspect that wouldn't have helped my situation. I turned off "Smoothing" and turned the "Line/Arc Tolerance" up to 60% and that was the fix. Nice clean Arcs now. This was a OE (operator error) 

So what is that "Smoothing" option even useful for?

Sorry for the delay in posting, I'm a noob so they limit my posts till i get my 10 post street cred.

The "Smoothing" option is great when you "don't want" Arcs. This is true when you are using the "High Speed Look Ahead" options on your machine control. With the High Speed options turned on, the control will do much better with "short line segments", since it can better predict the "acceleration and deceleration" needed to speed up and down better.

 

 

[nickbe10]

17 minutes ago, TerraXJ said:

So what is that "Smoothing" option even useful for?

I have only had to resort to "smoothing" a couple of times. Sometimes badly trimmed surfaces will give a little "hiccup" when going across the line.

I use Blend a lot and this toolpath seems (to me at least) to give fewer problems with this. On the couple of times it hasn't (making swaging dies so mostly straight lines with some fillet blends) I have used smoothing to calm the hiccups, but it does add code quickly.

[Leon82]

I did this for a part with a bunch of elipse. I put the tolerance at .0001 and the upper left  slider all the way to the right.