What's new
What's new
By:
Advanced search…

3d surfacing challenges, your best guess at this prob

L

LouGold

Plastic
Joined
Jul 14, 2021
So, I have successfully surfaced this with a 1/16th ball mill a couple times. All the other times is comes out like this photo attached. Really fuzzy and raspy on the flats.

I am running it at MAX rpm for the mill (11,500. I know 20k or 30k would be better but aint got it.) and at about .0005 IPT chipload and .0035" stepover, attempted with both scallop and raster(parallel) toolpaths. Tried with both 2 and 4 flute endmills and only had success a couple times.

A few questions I have are, given the 3d shapes, how much should I leave for the ball? I've been trying .003 before the final pass but should I do more? .010 or .012? Im stumped... Tried everything.. Maybe more chipload?
surf finish.jpg
 
hard to tell from the pic.
tool could be way out of balance or maybe youre recutting the chips.
what doess your coolant setup look like? relative to how much material to leave for finish....what material are you cutting? are you able to cock the tool or work piece over on and angle so that you aren't using the zero velocity portion of the tool?
 
Looks like a broken tool (or really bad grind on center) from here. Some of the shiny spots appear to be where it changes tangency and cuts on a different part of the ball.

If that happened here, I would say with certainty it's a broken tool. Sometimes tools that appear to be good start leaving fuzzy finishes, and we toss 'em. Like allout says though, there are so many variables it's hard to tell for sure.

Also, I've never had a ball want more chipload for surfacing. The folks who get really nice finishes running 40k spindles are rarely feeding fast enough to keep the chipload high.
 
Are you roughing this with the equivalent sized ball mill prior to the finishing pass? It appears to me that the tool plugged up, as would happen if it had to clear those deeper details with too much stock remaining from the previous toolpath.
 
The previous "semi finish" tool is a .250 ball mill, leaving like .003 stock everywhere... I am using a brand new ball mill every time to try and finish and it keeps looking like that...

its 1018 steel.
 
Rough it a bit closer, .001" should work better and increase the chipload a bit, maybe .002" to start
 
007Rob said:
Rough it a bit closer, .001" should work better and increase the chipload a bit, maybe .002" to start
Click to expand...

Id try going close like this too. Roughing with a 1/4 tool is probably leaving a lot in tight corners. I would rough it really close with the 1/16 tool, then do a final finish pass with a brand new 1/16th tool.
 
pretty obvious IMO whats going on here. you dont have enough SFM, or chipload is too high for cutting so close to, or on the bottom of the ball. the fact that it only looks bad where its near the center is a dead giveaway.
drop your feed, look into a ball mill with one flute going past the center.
also if you're using a larger than 2 flute endmill, your chipload is not accurate when you get close to the center since the geometry only allows for max of 2 flutes on a ball mill.
 
LouGold said:
The previous "semi finish" tool is a .250 ball mill,
Click to expand...

Could it be gouging? It seems to me that there is a lot of work for a 1/16 ball nose to clean up from a 1/4 ball nose. If it was me I would probably put an 1/8" ball nose as my semi finish after the 1/4 and then follow up with a 1/16 after that.
 
Ball endmill is clearly chipped/broken.
fixes have already been listed.
I favor prehard material for cutting consistency sake.
 
As some have said, the 1/4" rougher is too big to go right to the 1/16" finisher, use a 1/8" for semi-finishing. I'd leave a nominal .003", that feels about right.

What are you using for coolant, if any? What machine are you using, is this a proper VMC, or a router? What brand, coating, flute count and length cutters are you using?

Can you post close-up pics of a used cutter? It would be interesting to see its condition.

Agree with those saying tilt the plate and recode, but more than ~5-10 degrees may cause issues with some features depending on depth.
 
You might get a 10x loop and inspect your cutter bits, perhaps one bet vendor/name is better than another.

Failure to make a good end on a radius bit is a common error.
I used to know a fellow who finished ground carbide bits. He ground them by hand under a magnifying glass.
 
Milland said:
As some have said, the 1/4" rougher is too big to go right to the 1/16" finisher, use a 1/8" for semi-finishing. I'd leave a nominal .003", that feels about right.

What are you using for coolant, if any? What machine are you using, is this a proper VMC, or a router? What brand, coating, flute count and length cutters are you using?

Can you post close-up pics of a used cutter? It would be interesting to see its condition.

Agree with those saying tilt the plate and recode, but more than ~5-10 degrees may cause issues with some features depending on depth.
Click to expand...


Milland:

the coolant is a full synthetic (Called synergy I believe)

The 1/16 finishing cutter is always brand new before we start the finishing on a plate. I have tried 1/16" HARVEY 2FL balls, 4 flute balls, lakeshore carbide brand, redline tooling brand.

It is a proper VMC.. Its a Smart SM1165 (made by samsung) 12K spindle, but we're trying not to pin it at 12K for hours and running around 11,500RPM.

Milland, given your previous recommendations, What would you run for chipload on a 2FL ball, leaving about .003" stock to finish?

Thanks a bunch to everyone for your input!
 
2 flute PREMIUM endmills for finishing only. If you must go economical, OSG has a new series to compete with the "cheaper" tooling offered, and it works pretty good. Air-oil mist preferred, .001 stock to leave at MOST, .003 is way too much to leave for a .062 ball, I leave that much for .25 dia balls.
 
To add to what others have said earlier in this thread, I will suggest adding a re-roughing or rest machining operation(s) with a ball nose tool of the same size-or even slightly smaller-as your finisher. It can be difficult to visualize if you're unfamiliar with this sort of thing, but you can sometimes *think* that you have roughed/semi-finished your part to within the oversize value specified in these operations, but if you are using a larger tool, there is likely quite a bit more stock left in certain areas, and when your finisher sees this it can damage/break your tool quite easily.

Another thought: some (most?) CAM programs will have toolpath strategies that will automagically employ different strategies for surfaces depending on differences of geometry (constant Z for steep stuff, parallel plane or constant stepover for shallow, etc). In TopSolid this is called their "superfinishing" strategy; I have heard that Fusion has something called "steep and shallow" or something like that. I've gotta think that this is fairly commonplace these days, but what do I know? This might be worth a look, as it can save some programming work. YMMV as they say....

Good luck & have fun.............Brian
 
Some pretty good advice so far related to leave less stock for finish. No more than .001" when using a small cutter like a .0625" ball, light chip load of about .0005" per tooth, a stepover somewhere between .002"-.004", and always climb cut. Going back and forth (climb/conventional) is okay in something like aluminum where the geometry is handwork friendly, but if you don't want to spend time sanding and polishing the extra time spent ensuring every cut is a climb cut is recouped in handwork time. And make sure your coolant flow is more than adequate to flush chips and your concentration is high enough to lubricate things.
 
EmanuelGoldstein said:
I don't s'pose you could tilt the part a little so it's not trying to cut with the center of the ball ? If you look at the photo, on areas that are steeper you don't have that problem ...
Click to expand...

This. If you're perpendicular to the surface the tip of the ballnose will leave marks. Tilt the tool axis so that the cut is taking place further up the ball, not the tip.
 
You must log in or register to reply here.

Similar threads

3
Tips on 3D surfacing ABS-like plastic
Replies
1
Views
1K
Vancbiker
V








 

ABOUT PRACTICAL MACHINIST

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

Learn more about us.

STAY CONNECTED

Facebook Instagram YouTube LinkedIn Pinterest Twitter Tiktok

Register Become a forum member. Register today.

Sign Up Sign up for our e-newsletter.

© 2024 Copyright Practicalmachinist.com. All Rights reserved.

Back
Top