more on faceting

[k turk]

okay, i was just scanning topics and read about this and about two hours later it happens to me:

 

imagine you drop a pebble into a glass smooth pond, producing concentric waves - small and tight expanding to larger and elongated. now draw a containment rectangle from near the center where the pebble was dropped to the outermost rings and pull that surface out and put it in mastercam. the surface to be cut then is rectangular with a descending wave pattern.

 

i've cut the surface with a finish parallel toolpath with the tool running across the waves - ie up and down the waves as if surfing (for calis) or skiing (for canucks)

 

the surface on the elongated, further out waves is excellent progressing to an aztec temple quality finish on the smaller tighter waves. i have changed the filter tolerances; i have create arcs in all planes checked; and i have support arcs checked in the control definition. And, i haven't improved my surface quality.

 

CLUE? . . . the code in all of these efforts appears to be all G1 output.

 

any enlightening comments would be appreciated.

 

thanks

k

[3R!< W3NG3R]

What is your filter set to?

[k turk]

tried lots of bits - last settings

 

Filter ratio 2:1

Filter Tolerance 0.000333

Cut Tolerance 0.000167

Total Tolerance 0.0005

[Cad-Camr]

K, In your finish parallel parameters click on the total tolerance button. Select a filter ratio other than the default. This will make the rest of the page selectable. Chack all the boxes create arc xy yz etc. Now when you post you should get arcs. The faceting thing happens when your geometry is splines instead of arcs. This may me the whole problem. Fun Stuff Aint It!

[k turk]

Cad-Camr

 

yep, done that already . . . which is why i am puzzled about all the G1 code. i'm far from an expert on code, but it all appears to be line output . . . . . . . long shot, but you don't happen to know tom urban? a friend of mine who lives in eugene.

 

more info -

original file was solidworks.

running X2 MR2 SP1

[Cad-Camr]

Nope dont know Tom. I'm puzzled with the G1 thing to. Please post any info. Thanks

[BernieT]

Is the parallel toolpath running in a 0, 90, 180, or 270 deg direction ???

 

The arc filter for XZ or YZ only creates arcs in those planes.

 

HTH

[k turk]

yes, 90 degree. i will change it and report back.

[k turk]

opps, reread your post more carefully after being excited about promise for solution ----

 

yes, 90 degree. should be arcs, no?

[BernieT]

Yep

[k turk]

Anyone ..... anyone ... Bueller???

[Ralph@Faustson]

What is the approximate radius of the surfaces where you're getting facets? With smaller radi say .75 or less I'd be using .0001" tolerance. Also what size & type of cutter?

[crazy^millman]

Have you tried surface finish scallop with a bias angle of 45???

 

HTH

[k turk]

radii vary from approximately 2 to 0.5 and i have the total tolerance set to 0.0005.

HSS downcut ballend w/ 0.375 diameter.

 

haven't tried surface finish scallop. also thinking to rotate the entire cut 90 degrees and run the cutter along the waves instead of across. the customer took the part, but i want to track down the problem. i've had some less than stellar surfaces prior to this, and thought it might be a machine issue. the geometry of this particular part really highlighted how and where the problem manifests, but a solution is still in hiding. i am going to run some part tests with this surface next week when i have more time.

 

could this be a post issue? it is a 5 axis post, but only running 3 axis on this part. i don't understand why the code is all G1.

[Craig Madsen from CM3D]

Just for grins - turn OFF the arc filtering - I have found a few times when it actually affects the part quality in such a way as to make it worse, though the program is smaller with it on.

 

For that matter, try turning filtering off, - slows the operation at the machine, but the part quality may be quite a bit better. I have seen that type of response in several machining packages.

[k turk]

i'll try that as well and report back anything worth reporting.

[John Jr.]

It seems the only way I can get the faceting out is by using 2d swept but I cant use 2d swept for most parts.

[Rob Dusenbury CAD/CAM CONSULTING]

Lossen up your cut tolerance and filter tolarance. They are way to tight to filter anything. I doubt your machine can even hold a .0005 tolarence. Also I would be suprised if your 3d contour is even dimensioned tighter than +/- .001 even at that, you have a total tolerance of .002....A .001 high and .001 low.

[k turk]

you are right, the machine can't hold that tolerance. those were only the last settings i used in running the part - did several. i think the original total tolerance was set at .002. unfortunately, i kept overwriting rather than saving toolpaths so i can't say for sure. i know i just went smaller. interesting to try larger; i will give that a try.

 

also fuzzy on the relationships of total tolerance, filter ratio, filter tolerance, and cut tolerance.

 

thanks for the input

[k turk]

well for those who followed some of this.

 

i've run seven different toolpaths with varying parameters - finish parallel, tolerances high and low, arc filtering off, surface finish scallop on bias, and posted through my 5 axis and 3 axis post. very little difference on the gamut. the 3 axis version might be a hair better. i've copied a section of the code. they all pretty much look like this, with an occasional X move to jog the spindle over at the end of the run. does that look right? shouldn't there be some curve data?

 

;( TOOL - 08 )

;( T8_0.375 BALL / 5X_TT001 / ST2 )

N1250 M06 T8

N1260 M03 S15000

N1270 G00 X1.009016 Y0. A0. C0.

N1280 Z5.

N1290 Z1.591058

N1300 G01 Z1.341058 F30.

N1310 Y.043247 Z1.342406 F200.

N1320 X1.009 Y.100054 Z1.347276

N1330 Y.156507 Z1.3556

N1340 Y.21235 Z1.367341

N1350 Y.267375 Z1.382455

N1360 Y.321379 Z1.400886

N1370 Y.374163 Z1.422567

N1380 Y.425531 Z1.447417

N1390 Y.475294 Z1.475344

N1400 Y.523266 Z1.506245

N1410 Y.569271 Z1.540005

N1420 Y.613138 Z1.5765

N1430 Y.654705 Z1.615595

N1440 Y.703101 Z1.661354

[bogusmill]

If none of the usual suspects have helped it might be time to try the unconventional.

 

Have you tried flowline running parallel to the wave?

 

I see in your code A0. C0. Do you have a 4 or 3 axis post to try?

 

Convert the surface to solid or just for laughs and giggles project a line onto the surface/solid and see if it's arc's/lines or splines/lines. Maybe this might reveal clues to what MC is doing.

[HT]

How about change your ball dia. to smalller size like 5/16, 1/4 or even 3/16 ;Rotate your cutting angle 25.0 to 45.0 from where you at ;turn off your filter and set total tolerance to 0.0001

HTH

[k turk]

bogusmill - i've tried finish parallel running parallel to the wave . . again everything for the most part gave the same result. i remodeled the form myself (original model was an outside source) same result. nice idea; projecting a line onto the surface. projected entity analyzes as a nurbs spline. also, yes to your question - ran it through 3 and 5 axis post. i'll try a flowline path; i think that is one of the few i haven't tried.

 

no one has answered the question yet, so i'll go ahead and ask again. does the code posted a few threads up look appropriate for cutting along a wave? sorry if this is getting repetitive. i'm about ready to give up. it's just frustrating not being able to locate the limiting factor. i cut alot of three dimensional parts with curved surfaces and the result here was just not acceptable. could there be some factor in the post causing the faceting - ie limiting the output?

 

thanks again for all the suggestions

[BernieT]

Well, I have looked at your code posted above. 1st question - why 6 place decimals? 4 place should be plenty.

 

2nd, the Y movements are approx .05, the Z movements are approx .02 - no way you can get a smooth surface with such large movements. Either the total tolerance is way too big or your models surface is not smooth.

 

At this point I think you should call in your reseller to go over this problem with you. Something is wrong.

 

Sorry to not be more help.

[k turk]

bernie - 1st question - why 6 place decimals?

 

cuz i haven't thought to change it. agree, six is excessive, but haven't really give it any thought until you pointed it out. i seem to recall reading about adjusting that somewhere. is there a place value setting somewhere in the control definition?

 

 

quote:

_________________________________________________

At this point I think you should call in your reseller to go over this problem with you. Something is wrong.

_________________________________________________

 

is the implication that you believe something needs to be adjusted in the post?

 

and thanks, even small comments can be helpful. at the very least this topic is helping me bear down on 200 posts. i appreciate your input.