V carve inlay using tapered ball nose 5.4deg

[Aj6474]

Can any help with how to use a 5.4 deg tapered ball nose bit amana #4822-k doing v carve inlays. For the life of me i can not get the male to fit the female. I have tried adding the bit into different categories in the tool database and each one gives me different results but nothing that fits like it should. I have used the amana #45771-mk 30deg v carving bit with excellent results of a perfect fit plug. But i would like to use the sharper tapered ball nose for finer details on smaller detailed areas. My start/flat depths are as follows
Female start -0
Flat- 5.58mm
Male start- 4.06mm
Flat- 6.85mm
And these give me a extremely tight fitting plug but no matter what i try i can not get the same results using the 5.4 deg tapered ball nose. Can any please help picture of the v carve that i am happy with. But more than happy to change anything to make it better. I am using vectric pro and uccnc with a stepcraft m1000

[Aussie]

Try using a SD of 0.0 FD 6.0
Male (plug) SD 2.65 FD 4.85

Works for me

[Aj6474]

Cheers for that i will give it ago over the weekend while i am off work. Thanks

[ZipperHead55]

I have only used v-bits (usually 30 degree Kyocera scoring bit) and end-mills, so I'm not sure if the issue you are having is due to the depth of cut per pass you are using with the 5.4degree TBN. In my mind, you would HAVE to do those in one pass (ie setting DOC to 6mm, as per the female portion, and leaving that for the male portion (4.85mm). Otherwise, your sides will be "ridged" or jagegd where the bit cut down on where the first, then second, third, etc pass join up.

Maybe I'm overthinking it, but it seems that you would get better results (in general) using the v-bit (you can get down to 18degrees (9 degree angle) bits) approach, but I've been proven wrong plenty in the past, and if this method works, it does open up more possibilities for finer detail (in theory I guess, but once you get too fine, you risk chipping sections since they will be very thin. Nothing a little sawdust and glue won't fix though.

Allan

[adze_cnc]

I decided to draft out your settings and Aussie's settings for your posted sample. I also drew my potential setting based on the geometry presented.
 

00 png
 
The main differences are your setting gives a large gap between the pieces (the so-called "air gap") while Aussie's gives a lesser air gap but a potentially greater gap below the material (the so-called "glue gap").

I offer my take:

• socket: SD 0.00mm; FD: 4.17mm
• inlay plug: SD 2.65mm (using Aussie's value); FD: 3.00mm (good for a bandsaw blade)

One bonus is that you can use a thinner piece of material for the inlay plug.

I try never to assert that one set of settings will be of use in all cases because there are many different potential cases. Instead, I suggest learning how the various settings (and there are only 3—even then two of them could easily be set to 0). You can see an explanation of the at this post.

For what Aussie does those settings will work just fine. Having said that, your settings above would also work just fine for his projects. I'd argue that his socket flat depth can be much less than 6mm though as shown in the image above—this is apparent in your large flat area sample and not so much with letters and other finer details. Remember that the inlay (male) starting depth signifies the maximum amount of material to inlay into the socket. So for 2.65 and a socket depth of 6mm there could be 3.35mm below the inlay on larger areas.

But i would like to use the sharper tapered ball nose for finer details on smaller detailed areas.

...and if this method [using tapered ball-nose] works, it does open up more possibilities for finer detail

I'd argue that the 30 deg included angle cutter mentioned in the original can in many cases result in cutting finer details than the 5.4deg tapered ball-nose bit. The limiting factor here is the 1.5mm diameter ball at the end of the bit.

The following image shows the finest detail you can get at the full 2.65mm depth using Aussie's "canonical" settings. The 30 degree bit can go full 2.65mm depth for a detail that is 1.42mm wide. The tbn barely goes in.

If the 30 degree bit only cuts to a depth of 1mm you can get into details as fine as 0.62mm.
 

 
The minimum width of detail the tbn can get into is about 1.87mm at a full 2.65mm depth.
 

 

In my mind, you would HAVE to do those in one pass (ie setting DOC to 6mm, as per the female portion, and leaving that for the male portion (4.85mm). Otherwise, your sides will be "ridged" or jagegd where the bit cut down on where the first, then second, third, etc pass join up.

Two ways to avoid plunging to great depths are:

• use a manual method of creating "roughing" toolpaths to clear the extra material above the inlay plug (male) start depth. See this post
• use a gadget to automatically create the "roughing" toolpaths: such as the one I wrote and available at this post. The most recent version is on the 2nd page of the thread.

Can any help with how to use a 5.4 deg tapered ball nose bit amana #4822-k doing v carve inlays. For the life of me i can not get the male to fit the female.

One thing to overcome when using a tbn is an artefact on the inside corner of the inlay plug (male). See the following image:
 

 
One YouTube video I saw lambasts VCarve for producing this artefact. But, here's the thing, we're lying to the software when we create the tapered inlays. By choosing a start depth for the inlay plug other than zero we're saying to the software that there is no material above the start depth. The software then tries to get the centre of the tapered ball-nose bit to rise to the material surface at the vertex of that inside corner.

If the material is there we get the artefact. If it's not (as in the following image) everything looks just fine.
 

 
What he suggests doing is not using the V-Carve/Engraving toolpath for the inlay plug with a tbn but rather using a pocket instead. I can't remember if you need to do some offsetting of the vector artwork to accomplish this but it wouldn't surprise me.

I hope this is of some use.

Steven

[Aussie]

Yes Steven is correct.
For me I use a single pass only….DOC 7.5mm for the plug.
Chipping can be a problem for fine detailed inlays, I only use end grain and some hardwoods are better than others such as walnut, cherry, maple, yellowheart, osang orange, wenge etc
Timbers I avoid are oak, redgum, Blackwood
Hope this helps.

[Aj6474]

Wow all that information is amazing and really simple that even i can understand and all makes perfect sense. This is all new to me and i have lots to learn but with guys like you out there willing to help is amazing and will make the whole process so much easier. I think my best option is to just use the v carve bit and not worry about trying any more with the tbn. Thank you very much for the guidance.

[adze_cnc]

Ron does some pretty impressive works in end-grain wood and does use a tapered ball end bit to do so. I expect not one with 1.5mm diameter but rather one with a much smaller diameter (perhaps 0.5mm or even smaller), With a bit that small it can get into areas that the 1.5mm tbn can't.

The roughing pass gadget was written for those whose machines aren't sturdy enough to plunge at great depth through the material to get to the starting depth + pass depth of the cutters but would like to try their hand at tapered inlays.

It does have a bug (OK, error) in it that I should fix: on Vectric program versions 10.0 and above it doesn't remember the last tool used, Since I use v9.519 I don't see the error.