Engraving and Bit Creation

[cyberreefguru]

Hello everyone.  I've done a lot of searching and I can't quite find the answer to my question.  I'm doing some text engraving with F360 for the first time and the first couple attempts ended up with engraving that was not deep enough or wide enough (I'm using a 60 degree V-bit) Fusion is creating a path down the middle of the text, not around the edge like I've seen in some of the posts and video.  I read somewhere the tool is measured from 90 not to 90 (or vice verse), so I told Fusion my tool was 30 degrees instead of 60 and I started getting the correct depths and width.  Is this correct or am I just doing something wrong?

Secondarily, is there anyway to use engraving when the width of the font is wider than the bit?  I would think, and I have see it in videos, Fusion would follow the font outline not just down the middle.  Any suggestions would be helpful.  Thanks!

-Tom

[daniel_lyall]

Yep a 60 is 30 each side.

It all depends on the font and the tool size A engrave (also called V carving) is meant to go down the center of the text so it can do the V.

What it shows on screen and what is cut is different the below pick is a simulation, it is shaded with visible edges

This pick is done with wire frame

The pick below is the wire frame view from the side what you can see is the engrave done with a 3 mm Vbit the first one on the left it is meant to be 2.5 mm deep the middle one is meant to be 5 mm deep 5 mm stock, they are definitely not cutting to that depth.

The last one on the right is a 1/4 inch set to cut 5 mm depth. 

The top view As you can see the toolpath is down the center

now if we turn the stock on and show the text it does not go out side the letters in the simulation pick

So with the toolpath like this you cant go outside the letters.

this is with the letter's extruded

Now that I shown that. I know it's long winded But it showing you what you can do and not do.

How to get it to go out side the letters That is done by extruding the letters to a depth then useing trace and selecting the bottom of the letters I have left the text exploded it's same if it's not exploded.

This was done at 4 mm depth you can see where the tip of the tool was going file attached 

[cyberreefguru]

@daniel_lyall - thank you for the detailed response. I think I'm following what's going but my experience in the real world does not seem to be matching.

Assuming Fusion's taper angle is opposite from the manufacturer's designation, then my 60 degree bit should have a 30 degree taper angle.  Likewise, my 30 degree bit should have a 60 degree taper angle. Correct?

When I mill with a 60 degree bit I'm seeing good material removal.  When I mill with the 30 degree bit, I don't see much removal at all.  See attached picture.

The first two are 30 degree bit with taper angel set to 30 degrees.  #3 is 60 degree bit with the taper angle set to 30 degrees, which produces the correct results.  #4 is 30 degree bit with the taper angle set to 60 degrees, which I think is "right", but the results are a total fail.  I'm going to re-run the experiment to accurately record the setting and results, but I'm looking for insight.

As an side, is there a setting like F-Engrave that allows stock removal at max depth when the v-bit is smaller than the surface area of the cut?  I tried trace, contour, and pocket without the results I'm looking for.  I know Vectric V-carve has the feature, but I'm not looking to spend $300-600 for an operation I do 5 times a year.

Thanks!

[daniel_lyall]

What you can do is draw the tool.

Then extrude the text down 

Aline the tip off the tool to the center of the extrude side to side then move the drawn tool down to it touches the bottom of the extrude then flick the sketch over on it's side and turn wire frame on, then you will be able to visualize if the cutter can go deeper. 

The cutter can only go as deep as it's shoulder where the angle meats the shaft

Also you can just extrude the text through the model or as deep as you want and the tool will go as deep as it can fit just select the bottom contour and the bottom as the toolpath.

But this does not produces a V carve/engrave.

So in short you cant brute forces it, you can only go as deep as the cutter will allow in fusion.

[cyberreefguru]

I ran more tests and my results match the depth simulation but not width.  The 60d bit with taper=30 produces the size and shape as designed.  60d with taper=60 is too narrow.  However, 30d with taper=60 does not produce the size and shape as designed - it is (approximately) 50% too narrow.  30d with taper=30 produces even smaller results.  The real world results match the simulation from a depth perspective but not a width perspective.  The 60/60 and 30/60 simulation indicate the same depth exactly, and the 60/30 and 30/30 produce the same depth.  However, because the bits are vastly different, the real world width is not accurate for the 30d bit.  Again, I would think the 30d depth would be much deeper to achieve the correct width.  I have my bottom set at -0.125 from the stock top, and it's not getting anywhere near that depth.

I don't really understand the "align the tip to the extrude".  I can extrude the text and make the geometry the bottom surface or the bottom chain and that "fixes" the depth question, but does not honor the width in real life.  Unless I'm getting really lucky, only the 60d bit described as a 30d taper is producing correct real world results.

I'm confused.

-Tom

[cyberreefguru]

I ran more tests and my results match the depth simulation but not width.  The 60d bit with taper=30 produces the size and shape as designed.  60d with taper=60 is too narrow.  However, 30d with taper=60 does not produce the size and shape as designed - it is (approximately) 50% too narrow.  30d with taper=30 produces even smaller results.  The real world results match the simulation from a depth perspective but not a width perspective.  The 60/60 and 30/60 simulation indicate the same depth exactly, and the 60/30 and 30/30 produce the same depth.  However, because the bits are vastly different, the real world width is not accurate for the 30d bit.  Again, I would think the 30d depth would be much deeper to achieve the correct width.  I have my bottom set at -0.125 from the stock top, and it's not getting anywhere near that depth.

I don't really understand the "align the tip to the extrude".  I can extrude the text and make the geometry the bottom surface or the bottom chain and that "fixes" the depth question, but does not honor the width in real life.  Unless I'm getting really lucky, only the 60d bit described as a 30d taper is producing correct real world results.

I'm confused.

-Tom

[daniel_lyall]

Pick is off the tool settings, I am testing with, this is one tool I use It's a cheap as **** engraver, In the background you can see the tool is hitting both side's.

The width of the slot is 3.076  the tool is going down deeper than it should it does not produces a good result it is going down 6mm in to the slot this is selecting the edges not the text.

Now if you select the text it will only go as deep as it can to produces a good result, They are forcing it to look good.

Pick below is same tool but selecting the text not the extrude it's going down about 4.25mm and hitting the sides and it leaves a good finish.

 

The way vectric do engraving is V carving and it's 2.5D  it's not a smart toolpath it's all over the show what ever way you have it.

Fusion's engrave is 2.5D as well but they have added some smarts to it so if you select the text it will 90% of the time produces a good result, 50% of the time it wont be what you want at all.

As they have to cater to Metal workers as well, what don't need to go as deep most times and the engrave is near perfect for that, So us poor woodworkers have to find a balances between what looks good and what works.

I will think on this and ask for a improvement in the idea sation

[cyberreefguru]

Thanks @daniel_lyall.  I understand engraving from the bottom profile allows deep cuts and selecting the text allows contour matching.  However, what I'm seeing is Fusion is only matching the contour when I'm using a 60d bit described as 30d taper.  If I use a 30d bit described with a 60d taper, it does not match the contour at all.  That simply seems like a bug to me no matter how you slice it.  Regardless of metal or wood, it should still cut the proper width depending on the bit size, right?  Secondarily, I would really love some depth control with engraving.  Making one super deep cut does not produce the best results in wood, and I would imagine could generate disastrous results in metal.

-Tom

[daniel_lyall · Accepted solution]

@cyberreefguru you set the angle of the cutter per side if it's a 30 that's 15 each side, Fusion use's the whole cross section of the tool to produces the cutter image.

60 is 30 L side + 30 R side

30 is 15 +15 

that cutter image I put up it says 17.5 the cutter is a 35 don't ask why I put in 65 in the description.

@HughesTooling is that correct

The cutter may not quite go from edge to edge depending on the font used and it's size (this is a tiny amount a hair), the tail of the V should touch both sides of the font at the end of the font.

[cyberreefguru]

@daniel_lyall - man is that some sort of common knowledge in the CAD world or something?  It's completely not documented in Fusion that I can find.  Make a pretty big difference!  

So,

60 degree = 30 taper angle

30 degree bit = 15 taper angle

90 degree = 45 taper angle

Right?

[daniel_lyall]

No not realy it will ever be the angle of 2 side or 1 side. fusion use's both sides (i was told this my self over 2 year ago by the person I tagged for a double check) Vectric use 1 side.

with vectric if it's called a 60 you draw 30 that's when you make the tool image you draw half of the cutter.

When we get form tools in fusion it will be the same thing you draw half the tool and revolve the image.

I will draw you a pick when fusion gets it's head out of the clouds and does some work spinning it's wheels at the moment how rude

[daniel_lyall]

If you have a look at toolstodays web site on the V carve page have a look at the image and table, it shows where the angle is taken from in the pick below it's a 60 cutter as you can see it's the angle from side to side, If you lade one edge flat the angle would be 60.

To draw it in a revolve you would draw 1 side. what would be a 30 in the sketch revolve it you would have 60 from side to side.

[Anonymous]

I have a similar question.

I enjoy using the Engrave function to do script letters. The beautiful thing about this function is that it varies Z in order to fully cut the width of the character.

All works well until the width of the letter stroke approaches the diameter of the engraving cutter.  Then I experience something similar to the China Syndrome.

I have tried many workarounds.  It would be great if engrave had a rest machining option, one could cut the letter out with a square bottom cutter and finish corners and narrows with the engrave function.  But it does not have that option.

My last attempt was to do an offset in each of the wide sections and put a slug down the center of the stroke.  Then come later and cut the slug out.  Very time consuming.

Has anyone else experienced this problem? Anyone have an easier workaround?

Allan Steinkuhl

[Fueler]

Sorry Daniel, I could not resist.

"Fusion's engrave is 2.5D as well but they have added some smarts to it so if you select the text it will 90% of the time produces a good result, 50% of the time it wont be what you want at all."

sounds a bit Yogi Berra. "90% of the game is half mental"  or something to that effect.

[daniel_lyall]

There is a lot to engrave in terms of math, The math involved is over most peoples heads there are a few ways to do it, Whats in fusion is just one way and they are trying to cover all metal workers, And are trying to please wood workers.

The other program I use with V carve in it is for wood workers and it's quite different to how it is in fusion, you have a lot more control over what and how it cut's.

@Anonymous what you can do is use the traces toolpath to do what you wont, but you would have to draw in the corners, It would not be easy to do but it's not impossible, you wont be able to use a stick font.

what you can do is put your text in explode it, extrude it down to the depth you wont, do a offset sketch (turn chaining off) and just pick the ends of the letters then project them down to the bottom of the extrude.

then draw a line from the end of the line to the corner in your text that will give you a path to use for tracing so you still get the engrave look and you can have a flat bottom.

I will put up a example soon. 

[Steinwerks]

@curtis.chan made a video about this:

[daniel_lyall]

@Anonymous Is this what you wont I need to play a bit more it's just drawing the engrave toolpath, I just need to work out what offset to use to get sharp corners