I want to v carve some letters with a 60 degree v bit. The letters are 0.02735" wide. Im wondering if there is a list or calculation that will tell me how deep i need to cut to carve the letters out in one pass so it leaves one nice line. Has this idea become a reality?
As long as the width of your letters is less than the width of you bit, there is nothing to worry about. If the depth still needs to make several passes, the software accounts for that.
1 Like
Hi Nick,
A simple calculation for 60 deg. bits:
width at top * .8662 = depth
So:
.02735 * .8662 = .0237
1 Like
Thanks for the reply and i get what you are saying.
Let me rephrase the question.
If i start with a small depth with a 60deg v bit and it makes several passes which leaves a couple high spots in between the cut lines then how do i know how deep to go(max depth) to make it cut one solid line without going wider than the finished line should be?
Hope that makes sense
Wow if that works then thats very helpful. Thanks
What CAM software are you using?
Its carveco maker used with onefinity x50
Can’t you just input a depth that would be deeper than the tool will go if staying inside the lines?
Pat
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.
This is true for a tool with a “infinitely sharp” tip. Outside of that being physically impossible it would also make a horrible cutting tool as it would have 0 surface speed and flute volume at the tip. It would also be infinitely weak at the tip.
That being said the ratio works but you should be accounting for the tip. Here’s what they are for some common tip diameters at your 0.02735" wide cut.
-
0.005" tip diameter = 0.0194" depth
0.010" tip diameter = 0.0150" depth
0.015" tip diameter = 0.0107" depth
The simple way to do this by hand is to take your desired width, substract the tip diameter, then times it by the ratio. There are also multiple calculators online that will do it for you.
While I’m here, here’s the ratios for common angles.
-
30° = 1.866
45° = 1.207
60° = 0.866
90° = 0.500
What I believe they are trying to get at is that with a proper CAM solution you don’t really need this. All these calculations would be done in the software. The thing that could be hurting you is if you are not letting the software calculate it for you. e.g. if you have a defined width of the letter and force it to cut shallower than a single pass cut it will take multiple passes to do it. Alternatively, if you have a tool improperly defined (0 tip diameter) it will do all kinds of incorrect things.
Hope that’s useful. Let me know if there’s something I can expand on or help with.
2 Likes
You are making this more complicated than it actually is.
A V-Bit will not go any lower than the lines will allow. If you set a depth of 3/4 inch, but the lines are close together, the bit will stop at the lines.
If the distance between the lines is larger, you can set a start depth and the bit will never go lower than the start depth.
1 Like
This is something else i was curious about.
If it knows what bit i am using and the line is not very wide. I was wondering if i make the final depth a value that i know will be more than i need to fill the width of the line would that work.
It sounds like you are saying that it will know that it doesnt need to go as low as i have told it to go.
It knows what bit you are using because you told it what bit you were going to use. Using a different bit will not produce the same result.
Once the bit has touched both lines, it will not go any further down no matter what you tell it.