Need help cutting small letters

This forum is for general discussion regarding VCarve Pro

Need help cutting small letters

Postby highpockets » Fri Apr 29, 2016 4:20 am

I have a project where I need to cut some letters .2" and some .15" high. I'm using a 30 deg .125" engraving bit and "Kozuka Gothic Pro H" font.
I'm using Quick Engrave with a .02" depth, Outline. The .2" letters aren't too bad (could be better), but the .15" letters are completely wiped out on the inside areas.

Quick Engrave.jpg


I hate to reduce the depth of cut much more, but I think that's what I'm going to have to do.
Any suggestions on a better font or technique would be greatly appreciated.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby FixitMike » Fri Apr 29, 2016 4:41 am

I always use the VCarve toolpath for small letters. (Except for acrylic) I'm not sure what you mean by an engraving bit. Your description sounds like what I call a router bit.

Note that the VCarve toolpath does not work with single line fonts.

The Quick Engrave toolpath is intended primarily for a drag tool, which usually has a spring loaded diamond tip that basically scratches your material. When it is set for the outline using a V bit, the result is the same as when you use the Profile toolpath On the vectors.

For information on how the toolpaths work, see Help--Help contents.
Good judgement comes from experience.
Experience comes from bad judgement.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1205
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Re: Need help cutting small letters

Postby highpockets » Fri Apr 29, 2016 4:54 am

The cutter I'm using was purchased with the following description "30 degree tip angle carbide bits used for scoring or engraving"
It's just a sharp pointed router bit.

I don't want to V cut the letters, just outline them. Profile and Quick Engrave seem to do the same thing.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby highpockets » Fri Apr 29, 2016 5:03 am

Here's the lettering in question.
Attachments
Ring Box Top.jpg
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby FixitMike » Fri Apr 29, 2016 6:32 am

If you look at the geometry of a V bit tracing those lines, you will see that a 30 degree bit cutting .02 deep will cut a .01 wide line. Scaling the small text in the picture you posted, the middle of the e is .02" across, so if you cut along both sides, there will be very little material left.

I would suggest trying a single line 1L font such as Helvetica 1L.
Good judgement comes from experience.
Experience comes from bad judgement.
User avatar
FixitMike
Vectric Wizard
 
Posts: 1205
Joined: Sun Apr 17, 2011 5:21 am
Location: Renton, WA USA
Model of CNC Machine: Shark Pro Plus (modified)

Re: Need help cutting small letters

Postby martin54 » Fri Apr 29, 2016 11:29 am

If you are using engraving bits then they generally have a flat tip rather than come to a point, check to see if your bits have a flat & what size it is. You may need a bit with a smaller flat or even reduce the angle from 30 degrees to 20 or even 15 degrees. I have engraving bits in a range of sizes down to 10 degrees & with varying size flats.
As Mike says if the text is small & you are outlining it then the centres of letters is going to be very small especially if you are using lower case letters. You could also try reducing the feed rate which may help a bit.
User avatar
martin54
Vectric Wizard
 
Posts: 3277
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Need help cutting small letters

Postby scottp55 » Fri Apr 29, 2016 11:45 am

Sounds like one of Drillman1's 30 degrees.
http://www.ebay.com/itm/5-30-degree-angle-carbide-bits-for-scoring-or-engraving-2002-1181-030-/381608171704?hash=item58d99e98b8:m:m1h74lrvqIf354dF-_r296A
Try entering it as an engraving bit.
If it is a "Sharp" point then the flat size is .006"
If it's not specified then the flat is .012"
I always think in IPS, but you want to slow down for letters smaller than .18" to something like .5IPS X,Y, and down to about .35IPS for you Z plunge and around 17K for RPM. REALLY depends on your material though(those were hard Maple speeds).
Some fonts just aren't good for tiny stuff.
For tiny, I like Franklin Gothic Demi and have gotten legible down to .12" font height when VCarving.
Had good luck with 50/50 thinned Linseed or lacquer, and Watco natural and then carved twice an hour later....those bits really clean up the cut on a second pass.
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 2078
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Need help cutting small letters

Postby highpockets » Fri Apr 29, 2016 6:43 pm

Thanks for all the great suggestions. I'll try the different fonts. I'm also planning on trying the smaller text in Vcarve. Wish I could enlarge the fonts a bit, but the bride wants the Las Vegas sign big and their names and date small. The end product is a wedding ring box for the wedding ceremony in, you guessed it Las Vegas.

Thanks Mike, I'll try the single line fonts. Hadn't really thought about the groove with, that explains why the center of the letters are getting wiped out. May try a shallower cut depth for the small letters.

Martin, I may try finding some smaller angled bits. Where did you get the 10, 15 & 20 degree bits?

Scott, you nailed it. I'm using a Drillman1 30 deg bit with .006 flat. I'm just running on some MDF scrap right now trying to get some ideas on how things will turn out before I start working with the finish wood, which I believe will be Maple of something else with very little grain and is somewhat hard so it retains the detail.
Thanks for the feed suggestions. I'm running 30 IPM, plunge rate of 15 IPM and 16K spindle speed. Pretty close to your suggestions.

Wood suggestions would also be helpful.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby martin54 » Fri Apr 29, 2016 7:26 pm

I'm in the UK so not that helpful to you for buying bits :lol: :lol: I did just do a quick check on ebay & it looks like drillman1 does a 15 degree engraving bit, Scott might also know where else to get bits on your side of the pond.
As well as using a different font for the text or a single line font you could also try using all upper case letters which will look fine with a block type font. As for wood selection does the Bride want a light or dark coloured wood ?
MDF may be cheap so seems like a good choice when your practising but it takes the edge off of carbide bits pretty quickly so it can be a bit of a false economy in my opinion.
User avatar
martin54
Vectric Wizard
 
Posts: 3277
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Need help cutting small letters

Postby highpockets » Fri Apr 29, 2016 7:46 pm

Thanks Martin,

Had not thought about the MDF dulling the bits quickly. I guess it's time to make a decision on the wood and hit the wood store.

The bride showed me a light colored wood box so I'm sticking with a lighter colored wood.
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby scottp55 » Fri Apr 29, 2016 8:14 pm

Probably stick with hard Maple and run twice for fuzzies.
That's the only bit of his I had problems with the tip breaking.
Went through 3 in Bloodwood in 1 day, all at slow speeds.
The Onsrud 30 engraving with a .005" tip(spade type...keep RPM's way up) might be worth investing in.
It's my next investment, as I LOVE the 30 with the .01" flat,but not Quite small enough:)
scott
User avatar
scottp55
Vectric Wizard
 
Posts: 2078
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Need help cutting small letters

Postby highpockets » Fri Apr 29, 2016 10:46 pm

Thanks Scott,

Think I'll probably go with hard maple, need to go the hardwood store to pick some up.

You use a 50/50 wash of lacquer or linseed oil before carving to reduce the fuzzes and run the routes twice.

Doesn't this prevent penetration of a finishing stain?

Also I'd like to make the carved areas darker, either black or a very dark brown (leaning towards dark brown) to make it pop. Want to stick with a light stain for the box.

Suggestions on how to create this finish would also be welcome.

PS: when removing a 30 degree .006 flat tip bit from the router don't drop it on a concrete floor. It creates a tapered end mill. :oops:
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby scottp55 » Sat Apr 30, 2016 12:15 am

I always sand the tiny lifted edges off with 600G anyways, never stain...only an oil person usually, but Never noticed any unevenness in finish.
Usually get enough contrast just by the shadow and the endgrain of the cut soaking up more finish.
Lots of other good advice on infilling with paints and Gel stains on the forum,but never used them yet.
OH, when going that small/shallow, REALLY a good idea to surface with your machine and then sand to finish grit BEFORE carving.
Like I said, we finish in hand rubbed oil/beeswax, so that's 600G for us.
Maybe someone else can chime in with a good thread for infilling an outline?
Here's some pics done with the 30, some while experimenting,and a couple where I slowed it Waay down(especially Z) after learning better.
scott
Attachments
Bloodwood engravingbit .012flat 2 passes left side.jpg
EBONY STRONGBACKED.jpg
Ky 30degree standard flat2.jpg
PUTZ 1 last side.jpg
DRILLMAN 30 AND .125 INCH DOWNCUT.jpg
User avatar
scottp55
Vectric Wizard
 
Posts: 2078
Joined: Thu May 09, 2013 11:30 am
Location: Kennebunkport, Maine, US
Model of CNC Machine: Shopbot Desktop 5.5"Z/spindle/VCP9

Re: Need help cutting small letters

Postby highpockets » Sat Apr 30, 2016 4:50 am

Thanks for all the help.

I'm still working with crappy wood, but I did stop working on MDF (Martin).

Scott, I took all your suggestions and I'm amazed at the lettering detail I'm getting on bad wood, can't wait till I can get some maple to work with.

I faced the wood on my CNC, marked location and orientation of the piece in the jig. I then took the piece off the CNC and sanded down the face to finished grade. I then used Watco Danish Oil finish, first Natural then Medium Walnut. After drying I sprayed on several coats of Bulls Eye shellac sanding between coats. I then put the piece back in the CNC and carved the graphics running each g-code file twice to clean up the fuzzes. Worked great. I lightly sanded then applied Watco Danish Oil Dark Walnut followed by two coats of shellac.

I'm no photographer, it looks better in person.

Ring Box.jpg
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1286
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Need help cutting small letters

Postby martin54 » Sat Apr 30, 2016 10:50 am

I'm not against using MDF lol, but I do always point out to people that it can dull bits. I buy my timber from a sawmill & it comes quite literally as slices of tree, I thickness it & cut it myself so it's always easy for me to find a scrappy bit of hardwood if I need to do any testing. The sawmill will thickness it & cut it into nice edged boards for you & at a pretty good price to but far to much of it ends up as scrap in their bin if you buy it that way :lol: :lol: :lol:

Looking at the picture Las Vegas looks to be a little to the right of centre, might just be because the last letter is an "S" though. Doesn't really matter because thats what the eye sees, sometimes being technically correct isn't always best, sometimes you just need to go by eye :lol: :lol:
The date could do with opening out a bit as the numbers run together a bit. It's tight already though I can see from the picture. Of course that is just my thoughts on it :lol: :lol:

You could try lifting all the text a little, the married that's in circles could be reduced in size a little as well as lifted, that would give you a little bit more room for the other text.
User avatar
martin54
Vectric Wizard
 
Posts: 3277
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Next

Return to VCarve - General

Who is online

Users browsing this forum: Google [Bot] and 23 guests