I just ordered a 30 degree 1/4 v-bit yesterday. While I was looking I saw it was also available in a 1/8 version which I didn’t know. I figured the bigger the bit the better and faster right? So I ordered the 1/4".
This morning I decide to get on my carbide create and play around with the tool paths for my clock I’m making.
Remembering the 1/8" bit I changed it from 1/4" shank to a 1/8" shank. The resulting picture looked the same then I noticed the time difference.
Doing the same job with the 1/8" shank instead of the 1/4" shank was 5x faster! WTH?
Instead of 15-20 minutes it was now 3 minutes! Of course I immediately look at the feed rate. Yes, the feed rate for the 1/8" was faster than the 1/4" so I made both the same and using the 1/4" still did not come near the time of the 1/8" bit. The only thing left is tool pathing? Why?
I guess I should have bought the ones with a 1/8 shank…
Are the stepover & depth of cut also the same? Can you share the file?
There are a few variables that will change job speed. Step over, depth of cut, feed rate. What are the settings for each of your bits?
I have found (and this may, or may not be the case here), that there is often a mathematical problem based on the width of the groove you’re trying to cut and the geometry of the bit. When factors are just right, CC will choose some very inefficient paths…and if you change the width of the groove even 1/1000th of an inch, it will correct it. Try modifying the dimensions of what you’re cutting (if you can) just a slight bit and see if that doesn’t resolve the issue. [EDIT] Also, pay attention to depth of cut — if you are off by just a bit, CC will add a pass to make up the difference…For example, if the depth is .21" and you have DOC of .1 — you are asking for 3 passes — if the DOC for the other bit is .105, you’re only asking for two. Make sense?
- Gary
I actually did not think of that so I checked at was recommended which brings up another question.
Why would the recommended depth per pass for a 1/8 bit be larger then the depth of pass for a 1/4" bit?
Yes, you hit the nail on the head with that one. I was just experimenting and didn’t notice the depth per pass difference. So not only was the feed greater for the 1/8 but the depth of cut was greater too and thats what I really would like to understand.
Yes. So on the last pass its cutting the remainder and its only 1 pass difference. I don’t do it all the time but I do normally try to set the dpp evenly.
I took a second look at the recommended settings for the 1/8" bit and the 1/4" bit.
The recommended settings for the 1/4" is actually slower and the dpp is actually much less and that is the reason one was cutting much faster.
So why would a 1/8 bit have settings to be faster the 1/4"?
Its not necessarily my settings. It is the recommended settings. I can always change them I was just wondering why the smaller bit has faster recommended settings?
I suppose there could be a couple of reasons…perhaps the bit isn’t made for the same material (maybe like a foam-cutting bit vs. a wood cutting bit), perhaps the number of flutes makes a difference? (Someone would need to confirm that for me, I don’t know if it really makes a difference) - maybe you’re pulling the settings for different materials?
Nope. No material is taken into account. This are the recommended settings. Weird. Just thought someone would know.
Where did you get the settings? What brand are they?
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
First, I have to agree with Gary here. Need to know the tools and and where you’re getting the settings from for a specific answer to your question.
That being said most of it depends on geometry. I’ll give some examples below. Although, in general “V” cutters are not going to be bigger max diameter = stronger/faster. Like for like, at the same cutting depth, they will have the same mass and strength from tip to cutting depth.
All the below assumes everything else in the tool is the same other than shank size and the specific geometry feature being discussed. We’re also assuming that no other limit is being hit.
Tip size:
The diameter of the tool at the tip will greatly effect how fast you can cut with it. This is due to multiple reasons from raw material left in the tool, to surface speed, to flute volume (room in the tool to hold cut chips). Tools with “infinitely” small tips are also “infinitely” weak, 0 flute volume, and 0 surface speed. Basically the bigger the tip the faster can feed.
Helix:
This is the twist of the flute in the tool. This changes things in multiple ways too as the greater the twist of the flute the more shear you will get but the closer the flute are to each other reducing the amount of material left in the tool.
This also changes the force direction and the flow of the chips. An up-cut tool will have the least force and flow the chip up and out of the material. A down-cut will force the chips to the bottom making a harder time for the tip where there’s less flute volume.
There are also 0° helix tools (sometimes called straight flutes). These increase the cutting forces as the entire length of your cut is engaged at the same time.
The helix is basically a mixed bag and depends on the rest of the geometry and the material being cut.
Rake:
This is the angle of attack of the flute. The higher positive rake you have the less force it takes for the cut. But the weaker the edge of the flute. So more rake will allow more feed until you have too weak of an edge for the cut/material.
Flute volume:
As mentioned before this is how much cut material the flute can hold before packing. It comes at the cost of tool material though so it’s a balance of not more than you need being better and allowing more feed than too much or too little.
Tip style:
Some of the common versions of these would be flat/fishtail (not truly flat or it couldn’t plunge), corner break, radiused (bull-nose), and ball-nose. These are have varying effects on the forces, tip rake, chip form, and tool strength. So it’s a mixed bag feed wise. Assuming again that everything is “like” it would still be dependent on material. If my hand was forced I’d rank them most to least feed as corner break → radiused → fishtail → ball. This is mostly due to limits of flute volume balanced against weakest part of the tool and chip form.
There’s more than just these but that’s some quick examples.
Some other things to check for when comparing “V” cutters that could effect feeds:
Spade style cutters:
They look like a “cone” with half the cone ground away (hopefully at an angle starting before center). Then the edge is ground on one side the the other side is a different angle that doesn’t actually cut. They are typically low rake and 0 or low helix/flute volume. They are often confused for 2 flute cutters too which can make it more confusing.
Type of angle:
In general most of these will be listed by their included angle. However, they can also be listed as the draft or half-angle. I’ve seen places that swap them depending on intended application.
Hope that’s useful. Let me know if there’s something I can expand on or help with.
So, I guess that means that there is no way a 1/8" bit should be faster at v-carving than a 1/4" bit?
Since I have a router, I am in no hurry to speed things up and I normally just follow the recommended settings that I downloaded into my library. The info comes from a spreadsheet from IDCwoodcraft and it didn’t make sense to me when I compared the two together.
A complete V carving with pocket-clearing operation might be faster with a 1/8" rather than 1/4" tool if the 1/8" tool were able to clear more area than the 1/4" tool was, since the areas which weren’t cleared by the square tool are cleared by the V tool which takes a long while.
Sorry for the delay. Didn’t see this until Monday and I’m almost always swamped on Mondays.
No, any of the changes I listed above could make the 1/8" “faster” than a 1/4". I’ll use the 2 you are looking at using with the above to try and explain.
Looking at the IDC pages here’s what info I can tell of the tools.
1/4" shank
- Tip size 0.005" (0.13mm).
- Single flute.
- Guessing flat tip from the pictures but hard to tell.
- Some kind of helix but again no good picture to guess at what.
- Listed chipload: 0.0013" (0.033mm) (35IPM @ 27KRPM)
- Listed depth per pass: 0.025" (0.64mm)
1/8" shank
- Tip size ~0.0113" (0.029mm) from pixel measuring one of their pictures. They don’t list it anywhere I could quickly find.
- Single flute.
- Spade style cutter.
- Probably a flat tip.
- Probably zero or close to zero helix (generally true of spade cutters but no side picture. They also don’t have the “flat edge” comment from the 1/4" page).
- Listed chipload: 0.004" (0.102mm) (40IPM @ 10KRPM)
- Listed depth per pass: 0.15" (3.81mm)
Assuming the above is correct the limit of the 1/4" is probably the tip size. 0.005" is easier to choke. They also list a 20% step over for both. Depending on how the cutter is defined (with or without tip sizes) that could also greatly increase the cutting time of the 1/4" if you have anything but single line cutting.
From the other features, the 1/4" will give a better cut of the 2 though. If I was going to try and get more out of the 1/4" the safest bet would probably be by the cutting depth. If you try to increase the feed too much you are going to choke the tip and break the tool. I don’t know enough about these tools to comment more on the feed and speeds (nor would I regardless due to previous listed bias).
Just to be clear, I’m not endorsing these feed and speeds / chiploads. They are just what’s listed on their site. I’m personally an advocate of testing for YOUR machine and YOUR material regardless of the tool source and documentation.
Hope that explains it a little more. Let me know if there’s something I can help with.
This topic was automatically closed after 30 days. New replies are no longer allowed.