Tapered ball mill

This section is for useful tips and tricks for Aspire

Re: Tapered ball mill

Postby ger21 » Wed Feb 21, 2018 1:22 am

The big difference is that you can often skip the roughing pass when using a tapered ballnose, which saves a considerable amount of time.
Gerry - http://www.thecncwoodworker.com
Vectric Wizard
Posts: 1502
Joined: Sun Sep 16, 2007 2:59 pm
Location: Shelby Township, MI, USA
Model of CNC Machine: Custom DIY

Re: Tapered ball mill

Postby kaetamer » Wed Feb 21, 2018 4:27 pm

martin54 - I did, in fact, find a setting error which significantly increased cutting times w/the TBN. Once corrected, cutting times are comparable to SBN.
ger21 - I was aware of possibly omitting the roughing pass but some of my carvings are quite deep - not sure I'd want to push the bit to nearly its DOC - or am I being too conservative?

Thanks to all for info.
Vectric Apprentice
Posts: 28
Joined: Mon May 12, 2014 3:10 pm
Model of CNC Machine: CNCRP Pro 4824

Re: Tapered ball mill

Postby Leo » Wed Feb 21, 2018 4:47 pm

There is no specific toolpath for a specific tool. Only 3D, pocket, profile - etc

The software (vectric) will calculate the toolpath based on the shape of the cutter (tool) as it is described in the tool database. The radius on the tool tip as well as the tapered angles on the tool are calculated into the toolpath.

Sooooo - the tool data base needs to be set up correctly for the specific tool
Imagine the Possibilities of a Creative mind

User avatar
Vectric Wizard
Posts: 2971
Joined: Sat Jul 14, 2007 3:02 am
Location: East Freetown, Ma.
Model of CNC Machine: 1300 x 1300 x 254

Re: Tapered ball mill

Postby scottp55 » Wed Feb 21, 2018 5:14 pm

I regularly cut without a roughing pass IF!!!! I carefully inspect the toolpath and only see ONE plunge AND ONE lift!!
If the center of the model is a high spot, I'll do an offset toolpath if the first plunge is .125" or less.
If rastering, I'll ZZero...move the bit up so first plunge is only about .125"...Re-Zero Z...cut a few lines...stop and move Z down in stages until I'm at the original ZZero.
In both those cases, you're only cutting the stepover.
Check the file CAREFULLY though!!!
If for instance the model depth is .5", AND my LOC is .5"....many times I'll change the model height to say .47"...Inspect, and cut away.
I'm a smaller stepover guy though as I hate toolmarks as much as sanding :)
These were all carved with the smallest Chinese TBN with no roughing and medium to pretty dense woods.
9.12.17 CHERRY LION BOTTOM 1.5,1.5,17K 3% OFFSET CLIMB.jpg
9.13.17 DRAGON UNTOUCHED 1.jpg
User avatar
Vectric Wizard
Posts: 3133
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: ShopbotDesktop 5.5"Z/spindle/VCP10

Re: Tapered ball mill

Postby martin54 » Wed Feb 21, 2018 10:47 pm

ger21 - I was aware of possibly omitting the roughing pass but some of my carvings are quite deep - not sure I'd want to push the bit to nearly its DOC - or am I being too conservative?

I have always been way to conservative with my settings so I am the last person to ask but if you feel that omitting the roughing pass is not a good idea with the depth of a particular carving then you could run just part of a roughing pass :lol: :lol:

Toolpath the roughing pass & then run it until you reach a point that you are happy to switch to the finish pass & then stop it, have done that myself a few times once the roughing pass had removed the bulk of the material & I felt I could safely cut the finish pass without breaking the bit :lol: :lol: :lol:

Just make sure the cutting edge of the tool is long enough for the material you have left to remove which it should easily be as TBN bits tend to have quite a long CEL from what I have seen :lol: :lol:
User avatar
Vectric Wizard
Posts: 4661
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Tapered ball mill

Postby Xxray » Wed Feb 21, 2018 10:55 pm

Any 3d toolpath will require more time than 2d due to the increased z movement and shear volume of lines in the tap file.

Time saving options are, as ger21 pointed out, skip roughing [I often do this but not recommended for deeper cuts in hard woods]. What specifically are "deep cuts" and "hard wood" ? Well, you learn that from experience and breaking bits. Tapered bits are tough but of course have their limits, skipping roughing carries risks.
Sometimes I compromise and only do, say, 2 roughing passes instead of the calculated 5. Can also calculate toolpath on a 45 angle which *can* greatly reduce the risk of stress and breakage [this only works with an uninterrupted toolpath from top to bottom, often 3d toolpath will jump all over the place then this won't work].

A risk free method to reduce cutting time is increasing line stepover.
For the finest detail you'd want 8 to 13% for a finish pass but you can often jack it up to, say, 15 to 18% without a perceptible difference the naked eye can see.
Go much further than that though, and you will notice a quality difference that gets worse and worse as the % increases.
Sometimes thats fine if you are only doing a rough ball shape or something but if you are doing the last supper, you want max detail regardless of time.

Finally, having quality bit makes a huge difference as to your final product and longevity of the tool.
I tinker with cheap made in china bits occasionally, by and large though I invest in quality tools for predictable, repeatable and quality results.

http://www.precisebits.com/products/car ... 250b4f.asp
User avatar
Vectric Wizard
Posts: 1967
Joined: Thu Feb 17, 2011 8:47 am
Location: MI USA
Model of CNC Machine: CAMaster Stinger 1


Return to Aspire - Tips and Tricks

Who is online

Users browsing this forum: No registered users and 4 guests