Vectric Customer

With regard to three dimensional component work; when is a tapered ball mill preferred over a typical "straight" ball mill?

Thanks!

When your model does not have deep near vertical elements that the taper will mess up
When you want a stronger, longer bit that can cut faster
When 3 flutes will provide a better finish than 2
When you don't mind spending a lot more for the bit
There are more....

So I gather that you're not keen on them then...

The KEY ingredient

A 1/32 straight ball nose bit will probably break. I 1/4" shank 1/32 ball nose tapered bit is VERY STRONG

MOST of the time, the 3D surface needs only the very tip of the ball nose - so all the stuff behind the tip (the taper part) doesn't really matter.

The taper ball nose can "easily" reach 1" but a straight 1/32 will reach maybe 1/4" if you are REALLY lucky.

Personally, I use tapered ball nose cutters a LOT. I have 1/32 - 1/16 - 1/8. I pay generally about $32-36 each ---- BUT - it gets better.

I did buy some Chinese Ball nose cutters. They were metric, but that does not matter at all, at all. They were a LOT less expensive and performed very well cutting brass. Wood should be really easy.

I posted my evaluation in here somewhere.

Yes I would definitely buy more of the Chinese bits.

And Yes I do use straight bits as needed.

Jerry...
I would say the opposite, I use them almost exclusively. I would only select a straight ballnose for 2D work with radiused bottom.

As Gary & Leo have said there are a number of different reasons why people prefer to use a tapered ball nose instead of a straight ball nose, I use them for some of the reasons mentioned above, despite the extra cost the fact that they are stronger, less likely to break & you can machine much faster especially in the smaller sizes makes them worth the extra cost for me, I use them down to 0.5mm diameter for small detailed models but can still run them at a reasonable feedrate

Like Leo I also use straight ball nose bits for some work, as with any bit selection it comes down to what I believe to be the best bit for the work I am doing, probably not always right but it seems to work for me

For 2d work I use straight ballnose bits. For 3d work at 1/16" and 1/8" diameter I use tapered bits exclusively. I use 1 degree tapered bits a lot and I have never had an issue where the taper of the bit has had any noticeable impact on the final product. You have to get very close to vertical for the 1 degree taper contact the side of the cut. If you're making precisely engineered components it's one thing, but if you're making artistic work it's very rarely an issue.

I also use the 1/8" tapered bit on moulding toolpaths when I'm making cabinet door profiles. Some of these profiles go very nearly vertical, and I have yet to see one where the taper has made any difference at all. The taper adds a lot of strength - I've made hundreds of doors with the same bit with no loss of quality.

Just a note on those Chinese TBN's Leo mentioned...1/8" shank, and only a .25mmR tip, and I've made 2 MASSIVE operator errors with them without them breaking:)
First I drove it into a solid Sugar Maple block full depth using an offset toolpath, and the toolpath was zeroed to the spoilboard, and I zeroed to top of material
THEN, in Walnut I zeroed to top of material, moved ZZ up and was cutting a few lines(not using a roughing toolpath), dropping the Z down in steps... and had a static "Burp" that lost all positions in a "Wolf" carving(the digger closest to the wolves) and it plunged and started carving .5" deep at 2IPS in X,Y,Z!...reset and then tried again and MISSED a decimal point
Amazed the bit survived all that and is still cutting beautifully.
Rugged little suckers
Just mentioning.
scott

Oh, static was my grounding wire inside hose had a connection come loose while I was cleaning behind machine...NOT a usual occurrence!

For scottp55 and/or Leo - where do you get your Chinese TBNs? scottp55 - I checked the website on the side of the container in your picture - it was a dead end.

For all - when using a TBN - do you use a tapered BN tool path or a straight BN tool path? My limited experience demonstrated the TBN tool paths are far slower and if it rarely matters with regard to the taper - can you use a straight TP and speed things up?
Thanks.

There is nothing like a tapered BN toolpath nor a straight BN toolpath.

You use a 3d finishing toolpath and select the tool you want to use (tapered or straight) and the software will compute the toolpath corresponding to the geometry of the tool you chose.

What are you calling a straight or a tapered toolpath?

With the same tip diameter, you can cut faster with a tapered BN, as it is far stronger as you can read in the first replies.

Could you explain better your issue so we can help?

What I was (clumsily) trying to convey by the terms "TBN tool path" and SBN tool path" are the tool paths generated by either using a TBN or SBN as the tool used to generate the machining tool path.

What I'm asking is can you use the tool path generated by a SBN tool with a TBN loaded into the spindle? Some of the earlier comments suggested the taper rarely interferes with the carving (except on true vertical walls); I'm wondering if anyone does this to benefit from the added strength of the TBN and by extension, shorter carving times.

kaetamer wrote:What I'm asking is can you use the tool path generated by a SBN tool with a TBN loaded into the spindle?

Why would you do that? Calculate your toolpath with the tool you will use. Using a different tool for calculation and machining will lead to a wrong simulation preview and unexpected results.

There are some specific circumstances where you may trick the software with a different tool, but you'll have to master it before using such workarounds.

No idea of the advantage you are expecting in this case.

Here's the link for short assortment ones I bought;
https://www.ebay.com/itm/262858413910?V ... 2858413910
As soon as I was sure I liked them, I bought another 4 pack, 2 singles with the .25mmR, and one of the 1/4" shank .25mmR tips(haven't needed to use that one yet).
They all appear and measured the same.
They DO cut beautifully!

I agree with LGM, plug in the proper measurements, and use it.
Time is basically determined by tip radius/feeds and speeds/and stepover.... a low Z1 and Z2 are important also.
Lying to the machine CAN be useful under certain circumstances, BUT get used to it with an accurate preview first!
scott

Thanks LGM and scottp55 for your help.

kaetamer wrote:What I was (clumsily) trying to convey by the terms "TBN tool path" and SBN tool path" are the tool paths generated by either using a TBN or SBN as the tool used to generate the machining tool path.

What I'm asking is can you use the tool path generated by a SBN tool with a TBN loaded into the spindle? Some of the earlier comments suggested the taper rarely interferes with the carving (except on true vertical walls); I'm wondering if anyone does this to benefit from the added strength of the TBN and by extension, shorter carving times.

I didn't really understand what you meant by this as I have never compared toolpath times for the different bits so I set about doing some experimenting, took 3 different models with various degrees of complexity & toolpathed them using the same size SBN & TBN bits. Using the same settings for both bits there wasn't any difference in toolpath time that is worth noting

If you are experiencing a difference in the time it takes with each of the bits check your settings, not just feed rate but also stepover & plunge rate, you will probably find there is a difference somewhere within the settings you are using.

So if you use a TBN then you should actually be able to machine faster as being a stronger bit you can increase the feedrate without breaking the bit. The time saved should be more noticeable on smaller bits where you would have to run a SBN bit much slower to avoid breakage, I run TBN bits down to 0.5mm diameter & a straight bit at that diameter would be way to easy for me to break