Question V-Bits tool data base

[Makingtoothpicks]

I may be using the wrong bits as my V-bit when vcarving. I would like to hear from
you that have more knowledge then I do. I have a set of in-groove engraving bits
from Amana tool. I think I have been using them wrong. I have them defined in
both V bits and engraving bits. I after a long time now think this is wrong. I believe
they are only meant to be used as engraving bits and not V bits. If anyone uses these
how do you use then. There appears to be no way to describe there width. I believe
this is an important measurement when doing V-carving of things as it is used to
determine how deep a tool can go. They have a odd and not true V shape.

I may not have said this in a way that makes sense so ask me and I will try to answer.

Don

[dealguy11]

The in-groove bits can absolutely be used as v-bits. I'm not sure what problem you're describing. The very first parameter in the Geometry section for a v-bit is "diameter". Just set that to the cutting diameter of the bit. You should be able to look up the diameter (or radius, just double) for each cutter online. I know the geometry looks a bit funky, often asymmetric, but many of the cutters only cut with one flute. For example, on the 90 degree cutter only the short side actually cuts.

[martin54]

Don, the main difference between a V bit & an engraving bit (generally speaking) is that a V bit comes to a point & an engraving bit has a flat at the end. The length of the flat will vary & isn't dependant on the angle of the cutter. The wider the flat then obviously the bigger the flat bottom on your engraving.

When a V bit is defined in the software the biggest mistake I see people make is that they use the shank diameter when defining the diameter of the cutter. The cutter diameter should be the widest part of the cutter which will be at the top of the V shape. The shank size is often much smaller than this but in the case of your cutting knives may be larger.
I would measure the actual knife at the top of the v shape & use that as the diameter for your cutting knives if you can't find any other info on the knives

[Makingtoothpicks]

Thank you for the replies.
I think the thing that had me bothered was the funny shape.
Then if you look and only one side is cutting then it makes sense.
I do not use the shank as the size. I try to use the numbers that
are listed for the bits I use. I think I am going to have to look
closer at the Inserts as I don't believe they list a dia.they list
an angle and a depth

Don

[dealguy11]

You can figure it out from the table with a little math, or just draw it and measure the drawing. For example, the chart for a 60 degree cutter says the profile is 7.5mm tall (.2953"). If you draw a rectangle .2953" tall and put the 60 degree angle at one corner, then trim off the extra, you find that the radius of the cutter is .1705".

90 degree bit is even easier, as the radius is equal to the height, so 5/32 is the radius.

[lfinsr57]

It's even easier than that. All of the Amana bits I've purchased were available for download in DXF. Import them into VC or Aspire and you have a measured drawing to work from.

Edited to add that I also use these bits since replacement knives are cheap in comparison. Unless you have a tragic accident and crash the tool into the work piece... DAMHIK

[Makingtoothpicks]

Dealguy11 you come up with 1705 Radius and I measured one with a digital caliper
and come up with .355 dia. I guess I was close. Thank you all for all the input.
I used Vcarves simulation to run a tool path on a 5 in letter to see what it does.
5in is to big to do in one run. I set the speed down and enabled the tool . It was
interesting how it went.

I think what was bothering me was how deep a v-cut plunges on some cuts.
I made some celtic designs and it was going way deep on the cuts.there
seems to be no way to control that.

Don

[martin54]

I think what was bothering me was how deep a v-cut plunges on some cuts.
I made some celtic designs and it was going way deep on the cuts.there
seems to be no way to control that.


Don I think a lot will depend on your machine & how deep the carving actually is, not sure as don't have the software on this machine but think the DOC set in the tool database is still used with vcarve toolpaths. Problem I have seem is that the default DOC is OK if you are doing just a shallow carving where only a part of the cutting edge is being used but on deeper carvings where the full cutting edge is being used the default DOC can be to much

If I am doing anything that requires a deep V carve then I edit the DOC for the v bit & reduce it to something I am happier with, takes longer obviously but I am OK with that

[Makingtoothpicks]

I will take this advice and see what I can get. I am about
to cut a couple more Celtic designs. Iwill post after I make
them. I never thought about DOC working on V cuts.

Don