Hi All,



I'd like to cnc engrave text in this oval sterling silver piece.

I used the Draw Sold > Text option to create a solid text and then boolean difference to recess it into the metal.

I plan on using a V bit to engrave the text.

1. Which CAM software would you recommend for this? (Fusion 360 is not possible as it is now a paid software). I use a Mac.
2. How would I program it so the V bit cuts in the middle of the text, creating a single, V-shaped furrow? The font is Bookman Old style.

Thank you in advance!
Gunter

That font is going to be problematic for your plan of cutting with a v-bit center of letters. A v-bit makes a furrow with a point at the root and it widens at the crest. This means that it would be better to use a "follow path" command and then control the bit depth to < half the narrowest part of the font so it looks uniform. The issue is the font is not even across the lines and you would end up generating overlapping construction paths. I do not have that font installed but the one below is similar in red, the black would be the construction paths to illustrate the issue. An end mill would work better for generating a flat bottom relief or find a font that is uniform widths or plan on a little clean up at the root which will have two peaks at some locations.

See below results from using native font tool in V-Carve. They have dedicated tools to alleviate the issue of centering

https://www.vectric.com/products/vcarve-desktop

@Grendel - thank you very much for explaining this to me - makes sense now.

Appreciate you taking the time to help!

@Grendel - I got VCarve Desktop and have been tinkering with it for hours & hours.

I used a 20 degree single flute bit and it works on wood but does go much deeper than I need as I can't seem to control the cutting depth . I used a vcarve toolpath.
My aim is to vcarve in metal and am wondering if you could advise if I should use another toolpath or vbit?

The effect I'm going for is this:



VCarve didn't have the font Bookman Old Style but I added it easily.. so the font's there, I just can't get it to cut a nice v section.

In the vcarve toolpath, if I enter a small flat depth but still use an engraving bit (v), it mills alright but the depth is flat not v-shaped.

Sorry for the bother!

Thank you in advance.
Gunter

The depth in vectric vcarve will be controlled by the space in the font allowing the bit to drive down to its depth.

So closing the fonts 2 walls down will limit the bits depth. Also changing the angle of the bit can have it hot the walls sooner a d limit the depth...

To do what you are thinking, you should have/use a centerline, or a stick font, then do an engrave to depth with a v bit...

We can look at adjusting your font to do what you want.

I'll look at the first file you posted...

We need the text you want and the dimensions of the bit you will use...

Hi Gunter.

Here is an example of a text with a 5mm recess.
The letters "Tw" have walls with a 20 degree inclination, milling on the contour with an angular cutter and selecting an island.
The letter "in" has to be modeled and engraved according to the model with the selection of the appropriate milling cutter as each wall has its own slope.

https://disk.yandex.ru/d/TEqG8MisVXH9rA

@BurrMan - Thank you so much for your help!
I attached the file with the text in Bookman Old Style.
I'm open to any bit you suggest but I'm currently using a single flute 20 degree V bit.
The height of the letters is 4mm and I'm open to the depth as long as it is clearly a vcarve.


Much appreciated!
Gunter

@WN - Thank you very much for your input!

I'm not entirely clear I understand though - the engraving I'm after is like "in" so I'd like the TW to also have a vcarve.

Gunter, Burrman is correct...the bit geometry is determining the depth so it can accomplish the run. That goes back to what I first mentioned about centerlines (stick fonts) rather than offset/uneven fonts. The use of flat depth will restrict as you mentioned but if you do not want a flat bottom that doesn't help you here. You could modify the font to be performed in different mill runs

@Grendel - thank you very much. Would you mind explaining how I would go about making the correct
stick fonts for this particular font - Bookman Old Style. Attached is the file I'm working on.

Much appreciated!
Gunter

Hi Gunter,
So 1 more thing to clarify...

In this post here:

https://moi3d.com/forum/lmessages.php?webtag=MOI&msg=10542.5

You have a picture of "this is the effect i am after"

So zoom in on the "T"....

That is not "a depth". That is a variable depth controlled by how far the 20° bit can drop into the pocket of the font at any given point.

For this, we need to adjust the actual geometry of the font/letters and then determine what you want to call "depth".

The other option mentioned is a stick font, or a centerline path on your letters. This can be an engrave with your vbit at a set, controlled depth. (I don't know vectric well enough to know whether a centerline engrave path can also be 3d (z values), to have a variable depth to the engrave.

But anyway, an easy way to achieve the centerline path, without modeling it, can be to generate a vcarve as is now, then you can run the gcode through something like gcode2dxf. This will give you the vcarve toolpath as centerline geometry. Now you can run your engrave at the desired depth on your imported centerline

single line stick font pack.

http://www.mrrace.com/CamBam_Fonts/

You could try Estlcam. With it, you can set the vcarve depth and also use a roughing tool to clear a large area first.

Martin.

@BurrMan - again, thank you for your time.

I completely get what you mean by "For this, we need to adjust the actual geometry of the font/letters and then determine what you want to call "depth"."
So if I were to use Moi3d, choose the Bookman Old Style font from 'Draw Solid', and I use say a 20 degree V bit, how would I go about creating the geometry?

Also, "But anyway, an easy way to achieve the centerline path,"
Could you please explain how to create a centerline path from text in Moi3d?

Thank you!
Gunter

@AlexPolo - thank you so much for the link to the stick font pack.

Is it possible to create a stick font from a True Font and if so how do I go about doing that?

Thank you!
Gunter

Hi Gunter,
I'll try to explain here, as a video may be too involved.

So I started by taking the text you posted then vcarving it.... (With no worries of depth)

Here is what it looks like from a top view:



And here in a 3d view: (Note the depth is all over the place)



Then I post the gcode for that toolpath. I run it through a system to create a dxf out of the gcode toolpath, then bring that dxf into MoI:



I did some cleanup. Rebuilding and joining etc.... (The dxf comes out as line segments, so I rebuild them into smoother splines. Maybe somemore time could be spent here)

In this file, I left the dxf line segments in as other colored styles, for reference

So why do this?

I can now use "Engrave" on the path. Engrave allows me to set a depth at the spline level.

I can also use MoI's Edit Frame and "Flatten" the geometry. An just do a flat engrave at a single depth with a Vbit...

Let me know if this is not clear...

Note,
If you are going to "Flatten" the toolpath geometry, you will want to EXCLUDE the little "V" tails on all the letters... Those are Z level entries and exits per a "VCarve" toolpath. They wont translate into a flat engrave (Unless you are doing the "3D Spline Engrave" I mentioned first. Then you want to use those...

So for this part:

"""""""""""I completely get what you mean by "For this, we need to adjust the actual geometry of the font/letters and then determine what you want to call "depth"."
So if I were to use Moi3d, choose the Bookman Old Style font from 'Draw Solid', and I use say a 20 degree V bit, how would I go about creating the geometry?"""""""""""

You want to model the font to control the depth "You want"...

I would model my tool (You said 20 degree, but didn't include the diameter of the tool)

With the model of the tool, you can determine the width at the various depths of the VCutter. Then you would go to each letter in your font text, and do the modeling to constrain your desired depth.

A combination of separation, offsetting\drawing and rejoining things at the proper widths to stop the VBit at the depths you want

We can get into this if you want\need to. It would probably be a great exercise for me and others to see various techniques to do this.

Also, Still want to see Grendel's Input here..... Monster!

cambam stick font link appears to be not working. (?)

Alternate:
https://cambamcnc.com/forum/index.php?topic=1557.0/index.php

- Brian