Small Fonts and Best Tool for the Job?

This forum is for general discussion regarding VCarve Pro

Small Fonts and Best Tool for the Job?

Postby Gaylon Raney » Sat Jun 30, 2018 4:09 pm

Had a few jobs now where they call for small fonts and they want nice or fancy fonts such as a nice cursive or such. I tried using a 90 v bit but its to wide for the cursive it kinda blows out or over cuts details that make it look fancy. I also tried a 30 deg engraving bit.... first of all it takes forever to do it like over an hour where the 90 v bit was like around 15 mins. also the engraving was not looking right as it looked like it didn't connect both lines like the v bit does so it didn't do right either.
So if anyone can say what are some good fancy fonts to use and the smallest size able to use? Is there such a thing as to small for font? I would think no but still new at this all. What is Best tool to use for small fonts and details? place to buy it so I can pick one up soon to get these jobs out.

Is there some fonts that are just unusable? Thanks to all in advance
Gaylon Raney
 
Posts: 11
Joined: Sun Aug 06, 2017 9:51 pm
Model of CNC Machine: shapeoko 3 XXL

Re: Small Fonts and Best Tool for the Job?

Postby Adrian » Sat Jun 30, 2018 5:30 pm

For really small stuff you're best to use the single line fonts and use a profile toolpath with a v-bit.

Sounds like you might not have had the toolpath or tool set up properly when you used the 30 degree bit. Most of them have flat bottoms. Did you set that up or just define it as a v-bit?

About the smallest I go with a V-Carve toolpath and v-bit (60 degree) is about 10mm. After that I go single line unless it's in a material that doesn't chip. I know some other forum users go a lot smaller than that though.
User avatar
Adrian
Vectric Archimage
 
Posts: 8520
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Small Fonts and Best Tool for the Job?

Postby martin54 » Sat Jun 30, 2018 5:54 pm

90 deg is not really the right bit for small text regardless of what toolpath strategy you are using, yes some fonts work better than others for small text & there are other things you can do to help machining, one font that I like is Shelley Volante but it has a very fine stroke width which often means that it won't carve deeply enough with a v carve toolpath even with something like a 30 deg 0.1mm engraving bit. I get round this by using a very small outline (offset) which makes the stroke a little thicker, practice will tell you what you can get away with before the font starts to look distorted.
Block fonts are generally best for small text but unfortunately they aren't very fancy :lol: :lol:
Other things that help is having a range of different angled engraving bits, I have from 10 deg to about 130 deg or maybe more. Flats on them make a difference to carving as well so some of them I have in a range of different flat sizes from 0.1mm to generally about 0.5mm but I do have a couple of 60 & 90 deg bits with up to 3mm flats.
Some other things that can help with machining small text, use a sanding sealer before carving, this helps to prevent chipping, slow the feed & speed rates down which can also help with chipping especially if your machine is not particularly rigid. Your machine would fall into the not so rigid class in my opinion.
Make sure you are using sharp bits, I would suggest keeping some bits just for small text if you tend to use v bits quite a lot, also try a forum search as it is something that has been discussed before.

Sure others will chime in with some useful info that hasn't already been mentioned :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3984
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Small Fonts and Best Tool for the Job?

Postby highpockets » Sat Jun 30, 2018 6:05 pm

Here's a pretty good thread on how to work with small fonts.
viewtopic.php?f=2&t=24839
John
Maker of Chips
User avatar
highpockets
Vectric Wizard
 
Posts: 1820
Joined: Tue Jan 06, 2015 4:04 pm
Model of CNC Machine: PDJ Pilot Pro

Re: Small Fonts and Best Tool for the Job?

Postby Gaylon Raney » Sat Jun 30, 2018 6:11 pm

martin54 wrote:90 deg is not really the right bit for small text regardless of what toolpath strategy you are using, yes some fonts work better than others for small text & there are other things you can do to help machining, one font that I like is Shelley Volante but it has a very fine stroke width which often means that it won't carve deeply enough with a v carve toolpath even with something like a 30 deg 0.1mm engraving bit. I get round this by using a very small outline (offset) which makes the stroke a little thicker, practice will tell you what you can get away with before the font starts to look distorted.
Block fonts are generally best for small text but unfortunately they aren't very fancy :lol: :lol:
Other things that help is having a range of different angled engraving bits, I have from 10 deg to about 130 deg or maybe more. Flats on them make a difference to carving as well so some of them I have in a range of different flat sizes from 0.1mm to generally about 0.5mm but I do have a couple of 60 & 90 deg bits with up to 3mm flats.
Some other things that can help with machining small text, use a sanding sealer before carving, this helps to prevent chipping, slow the feed & speed rates down which can also help with chipping especially if your machine is not particularly rigid. Your machine would fall into the not so rigid class in my opinion.
Make sure you are using sharp bits, I would suggest keeping some bits just for small text if you tend to use v bits quite a lot, also try a forum search as it is something that has been discussed before.

Sure others will chime in with some useful info that hasn't already been mentioned :lol: :lol:
Adrian wrote:For really small stuff you're best to use the single line fonts and use a profile toolpath with a v-bit.

Sounds like you might not have had the toolpath or tool set up properly when you used the 30 degree bit. Most of them have flat bottoms. Did you set that up or just define it as a v-bit?

About the smallest I go with a V-Carve toolpath and v-bit (60 degree) is about 10mm. After that I go single line unless it's in a material that doesn't chip. I know some other forum users go a lot smaller than that though.


Thanks Guys I'll keep it mind about the offset thats a good idea. on the 30 deg its not a flat it comes to a point just like the v bits so I ran it as a v bit should it be ran or set up differently?
Gaylon Raney
 
Posts: 11
Joined: Sun Aug 06, 2017 9:51 pm
Model of CNC Machine: shapeoko 3 XXL

Re: Small Fonts and Best Tool for the Job?

Postby martin54 » Sat Jun 30, 2018 9:28 pm

If your 30 deg bit comes to a point then if you have it set up as a V bit then that is correct, engraving bits which have a flat are entered as engraving bits & the set up includes a field for the flat dimension.
If your 30 deg vcarve toolpath showed correctly in the toolpath preview but machined a bit strangely then the problem is with the machine or the bit, possibly the bit is not actually 30 deg. If the toolpath preview didn't look as you expected it to then you may not have the bit set up correctly in the tool database. :lol:

With small text you can only use very small offsets, use the toolpath preview & adjust the offset until you have something that looks correct, to much offset & it will distort the font or just mix all the letters together so it just looks a mess :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3984
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)


Return to VCarve - General

Who is online

Users browsing this forum: No registered users and 24 guests