V-bit v Engraving bit

[highpockets]

I've always used a v-bit to create v-carve toolpaths and it works fine.
I decide to buy some engraving bits to, well, engrave on a placard. But I've notice a problem in the preview of the placard (haven't actually machined one yet).

Using a 30° v-bit

Using a 30° engraving bit

What am I missing?

[LittleGreyMan]

What am I missing?

Probably nothing John. I guess your text is very small and the flat tip doesn't have enough space.

With a conical bit, you can theoretically always engrave. In this case, the engraving of the parts which are missing with the engraving bit are probably very shallow.

[sseale]

Nit sure this is reason for the skipped areas but just a quick look at the Edit Tool setup I see the included angle is full angle for V Bit and for engraving bit they define the half angle. You have 30deg set for both. Are your bits both 30deg full angle?

[highpockets]

Nit sure this is reason for the skipped areas but just a quick look at the Edit Tool setup I see the included angle is full angle for V Bit and for engraving bit they define the half angle. You have 30deg set for both. Are your bits both 30deg full angle?

Thanks, I corrected the tool to 15°, but the problem still exists.

[martin54]

As has already been said it is quite possibly the flat tip on the bit not being able to fit, you could try reducing the flat tip size to see if it makes a difference, that would confirm it was the tip that was causing the problem

[scottp55]

John,
The flat just can't get into the narrow sections.
Now that angle is correct, you'll still have the same problem.
Copy one of your 30 degree VBit's and ignore the flat. just rename(I have my small tips entered as both for this type problem)
Gotta watch the stepover, and rpm's(single flute)

As an Engraving bit, stepover is a percentage of the flat size.
As a VBit, it's percentage of the shank on a full carbide.
I like to get at least 2 passes of the flat for sand free finish(use a decimal point in stepover,or plug it in).
EXAMPLE pic was setting for 1.1"inch Owl 3Ds.

For wood that you DON"T want to mess up use Michael T's setting I like(in IPS) .3(X,Y move speed), .3(Plunge speed), 18K will work in even splintery woods....IF I work a wood regularly, I sometimes go .4-.5, .35,18K.
Keep your Z1 and Z2 as low as you dare. IF surfaced yourself,sanded to finish,1 coat finish applied...usually my Z2 will be .02 with Rapid Plunge set.
I max at 18K for my spindle...if you have more speed you can increase after testing.
Preview will be off by approximately .002" on all sides, but don't see a problem with that font, except upstrokes will merge earlier.

TEST, but a good brushing, and quick 600G(if needed), and cutting twice if stiff/medium (Boar seems best) brush doesn't clean up first pass, usually meets even MY standards
Play with it until you get used to a single flute.
Good luck with the Lumieres:)
scott

(Hope I have you thoroughly confused John:)

[Leo]

I will also vote on the flat tip

The angle has nothing to do with it.

The text is tiny and requires a sharp pointy cutter.

[highpockets]

OK, Thanks for all the help. It turned out to be the tip was too wide at .004 I reduced it to .002 and it worked out just fine. I'll run a test piece and see how it actually engraves...

[martin54]

What I do with a lot of fine script fonts is to offset them outwards a very small amount to make the stroke width a little thicker, try it with a small offset to see how it looks, offset to much & the font will start to look wrong & your letters will start to run into each other so you need to take a bit of care
You might find you can't increase it enough for the flat to fit in some places at 0.004 if the text is very small but any increase will help as long as the font still looks good

[scottp55]

Try it as a VBit later John....Actually improves legibility as well.
Gotta get used to "lying" to your machine at some point for the rare circumstances. and you have enough experience to "Fib" a little like you just did
scott

[mtylerfl]

Specifying a small Start Depth is often a workable solution to get “fine” text to engrave/VCarve without blank spots.

[martin54]

Or you could simply laser engrave it John

[highpockets]

Or you could simply laser engrave it John

[highpockets]

Specifying a small Start Depth is often a workable solution to get “fine” text to engrave/VCarve without blank spots.

Michael, I've used that technique before using a v-bit, but using an engraver Aspire (and assume VCP) still refuse to cut the very thin lines.

[mtylerfl]

Hi John,

Can you post a sample file we can try for ourselves? What is the font you are using so we/I can make sure I already have it. I want to do an apples-apples Test. The sample file of yours will assure the same text size for the test.

(We May discover that only a pointed V-Bit will preview and cut correctly for the fine lettering.)

EDIT: I just read through the entire post from the top. Leo has already mentioned this may require a “pointy” bit. I agree. No need to post a file - I did a quickie Test with a fine script font and saw what you’re running into. Start Depth is little help for small, fine text using a flat tip bit...none really. To get it to cut without blank spots, the Depth has to be set far too deep to keep the text recognizable.