[Torontocnc]

Good day,

I am having trouble finding info on how to calculate a feed rate for a v-bit.

I have a 44.5mm(1.75") diameter V-bit ill be using to to do folds in 3/4 mdf. I was thinking of doing 1 pass at 6 meter a min. 1/2" shank at 15000 or 18000 rpm.

I did a rough calculation from some random guides I could find and found my chip load to be 0.007 or so. That is really low or I just did it wrong.

Should I do 2-3 passes? Use the 18000 rpm ? Or anyone know where I can find straight forward info not relating to compression bits? Or doe sthe bit type not mater?

Thanks as always guys,

Jordan

[JerryBurks]

At a first glance this sounds very fast and deep. Not sure what kind of spindle power and hold-down you need to do that.

I would start with several passes and a bit slower and work you way up.

At that speed you may also need a flattened tip because a sharp tip does not have any surface speed to speak of and is only dragging through the material.
I am not sure if you can cleanly calculate a chip load with a v-bit.

[Torontocnc]

Ill be using a 6-8hp router on a flat suction table. I think the tip comes to about .5 to 1 mm flat, maybe a bit more. I tried a few tests at 3 passes and 5M/min, worked fine, but like to speed up, but do not want to snap the bit.

[ger21]

As Jerry alluded to, the tip of a V-Bit is moving very slowly. So you actually have a variable chip load. It's very low at the wide portion, and extremely high at the tip, which is the weakest point of the bit.

We actually do a lot of miter folding with a single flute indexed carbide V-Bit. I think your 6m/min at 15,000 rpm is OK, but be aware that it will put a fairly large load on the spindle and machine. Taking multiple passes won't do much more than wear out the bit faster.

Depending on your machine, I'd stick with the 15,000 rpm and try anywhere from 3m/min up to around 8m/min.

[ger21]

Ok, with 8HP, you should be OK with a single pass at 5-6m/min. That's at least 3x faster than your 3 passes.

If you have an ER32 collet, I'd recommend an indexable cutter with a 19mm shank.

[Torontocnc]

Ok, with 8HP, you should be OK with a single pass at 5-6m/min. That's at least 3x faster than your 3 passes.

If you have an ER32 collet, I'd recommend an indexable cutter with a 19mm shank.

Well the bit was already purchased. 1/2 inch shank, but 2 flutes. Im more worried about breaking the bit then the wear. We have a one off job of folding, so sending in for sharpening isn't going to slow production much.

On the subject of folding, is there a better bit for it, or has a smaller tip? After I cut, there is a sizeable flat area at the base. Luckily that leaves a nice chamfer on the point, bit a large gap that needs a lot of glue on the inside.

[Torontocnc]

We actually do a lot of miter folding with a single flute indexed carbide V-Bit. I think your 6m/min at 15,000 rpm is OK, but be aware that it will put a fairly large load on the spindle and machine. Taking multiple passes won't do much more than wear out the bit faster.

So we were able to get a bit like you described in(CNC V Groove Miter Fold & Signmaking Insert Router Bit by Amana Tool). It worked great in terms of cutting, 8.89M/min at 18k I believe. But our problem was when we folded the material it either cracked the corner(at .3-.5 mm from surface) to bubbled and looked bad(.1 to .2 mm from surface). Not sure where the problem is. The bit comes to a sharp point as opposed to a flat. It is a 91 degree bit. What we had to do in the end is go with a regular v-bit, 2 flutes and comes to a bit of a flat on the bottom(V Groove Router Bits by Amana Tool). This leaves a approximate 1 mm flat at the bottom of the valley and leaves a larger chamfer on the corner. Also this leaves a large glue space behind the corner.

I would love to know how you guys fold with the sharper bit? Internet sources and previous out-sourced v-folds we have brought in used the sharper bit, but I cannot replicate them. We are cutting on a nesting table, so lots of support underneath and great hold downs.

[ger21]

What material are you trying to fold? I've gotten somewhat acceptable results with veneer, and barely acceptable with melamine. (had to lightly sand and touch up the edge with a marker). I'm assuming you're taping before cutting, right?

A week or two ago, while browsing WoodWeb, I read multiple posts from multiple people that said you really can't miterfold with a router. The reason is that the tip is spinning so slow, that it can't make a clean enough cut at the tip. This makes sense to me, and corresponds to the results I've gotten.

What we do when folding solid surface, is cut .03" (0.8mm) through the material, and tape together after cutting. We've also done this with oak veneer and achieved good results.

It appears that if you need to do a lot of miterfolding, you need to buy a miterfold machine.

[zool]

A thread on this issue from WoodWeb:

Making Miter-Fold Corners with Wood Veneer