Engraved text depth

[GUNNERNV]

 

I am having a problem with the depth of the text I am trying to engrave. I can only engrave part of the word even though I have change the depth of the cut. The machine keeps raising up and not staying at the intended depth. I have attached a photo. The text is supposed to say “The Middaugh’s”. Any help would be appreciated. 

[g-andresen · Accepted solution]

Hi,

While engraving, the depth is determined by the distance between two lines.
If you want to have a larger depth with an unchanged template, the point angle of the cutter must become smaller.

günther

[GUNNERNV]

How do I change the point angle of the cutter?

[HughesTooling]

Got to ask, with all the variation in depth of cut, how flat is the piece of wood? It looks like it's curved down near the bottom of each letter.

Mark

[g-andresen]

Hi,

---

@GUNNERNV wrote:

How do I change the point angle of the cutter?

---

this way:

günther

[GUNNERNV]

The wood had been planed flat and I had no issue cutting the groove into the piece. I can’t figure out why it has such a variation in the depth of the cut and that’s part of the problem. The bottom of the letters are getting cut correctly that’s why it looks that way.

[g-andresen]

Hi,

This is how the point angles of V-bits affect engraving:

günther

[HughesTooling]

---

@GUNNERNV wrote:
The wood had been planed flat and I had no issue cutting the groove into the piece. I can’t figure out why it has such a variation in the depth of the cut and that’s part of the problem. The bottom of the letters are getting cut correctly that’s why it looks that way.

---

Can you share the design with the CAM setup and OPs? Export as an f3d and attach.

Thanks Mark

[g-andresen]

Hi,

---

@GUNNERNV wrote:
I can’t figure out why it has such a variation in the depth of the cut and that’s part of the problem.

---

Depth variation is characteristic of engraving!

günther

[GUNNERNV]

Exported file attached.  If its missing something let me know.  Thank you for the help.

[g-andresen]

Hi,

Your file contains a special font that I don't have.
Therefore, it is not possible to create the engraving mode in a right way.
Select the font and convert it to curves after right-clicking and upload the new file.

Then we can transfer the contours correctly into the engrave process.

Once again: There are no constant depths in engraving.

günther

[g-andresen]

Hi,

---

@g-andresen wrote:

convert it to curves after right-clicking

means "Explode"

günther

[GUNNERNV]

Exploded text file attached.  

Thank you

Kyle

[HughesTooling · Accepted solution]

Now I see the font what you're getting is what I'd expect. Engrave uses 2 points of contact to generate the V Carve look. If we look at the e you can see on the left the V cutter can go quite deep but on the right the distance between the curves is small so the depth will be very shallow. And if you look at the apostrophe the cutter's going to go a lot deeper.  Your only option is like @g-andresen  suggested and use a more pointed cutter and maybe set a maximum depth so you don't go too deep.

You might want to use a 60° cutter. You actually call your cutter 60 V Bit but you've not set the angle correctly

[HughesTooling]

Another problem might be you have the stock top set to 0.04" in the setup, depends on how you've setup the datum on the machine.

[g-andresen]

Hi,

Please take a look at the screenshots.

1. with the text size, a maximum depth of 0.21 mm is achieved with a 30° V-bit.---  15° > max. 0.42 mm
1. There are some overlaps that need to be eliminated.

günther

[GUNNERNV]

Would it make sense to remove the .04 stock offset.  I don't recall setting up that offset when I created the stock.  I am also not sure how to edit the datum on my machine.  That wasn't part of the setup process I followed.  How do I eliminate the overlaps?  

Thank you,

Kyle

[g-andresen]

Hi Kyle,

If the offset reduces the milling depth, I would remove it.
The overlaps must be removed in the sketch, e.g. in Fusion or a vector graphics application.

günther

[GUNNERNV]

How do I eliminate the overlaps in Fusion?  I cant figure out how to eliminate the and still create all the chains.  

[g-andresen]

Hi,

I prefer V-Carve, but it can also be done in Inkscape.

günther