Help with Color Core Tooling/Toolpath

This forum is for general discussion regarding VCarve Pro

Help with Color Core Tooling/Toolpath

Postby johnelle » Tue May 22, 2018 10:51 am

Posting this question at the suggestion of support since they claim to know nothing about the topic (not sure I understand why but...)

I am trying to work with a two color plastic which in the US is called "Color Core" for the first time. Using simulation I have tried different approaches but none are quite what I was hoping for.

The manufacturer's recommendations are:
http://www.kingplastic.com/wp-content/uploads/2014/05/CNC-Engraving-King-ColorCore.pdf

I started trying to use plastic-specific end mills but Vcarve only allows those for "quick engrave" The Vcarve with V tool produces very odd results in simulation.

So far the closest I have come is using a 1/16" ball nose and a V-carve path. but the bottom is fairly rough and the edges have a little fuzz. Next try was going to be a plastic-specific square end mill and maybe a pocket path(?) if that is allowed.

Please recommend which path type and tool you think would be appropriate. I believe the letter edges need to be square (perpendicular to the surface) and the bottom should be flat. Cut is fairly shallow (0.1 in. max) because you are just removing the top layer to expose the "core" color.

Unfortunately this stuff is really expensive because of shipping so trial and error tries are limited.

Thanks.
--
John Ellenberger
Groton, MA
johnelle
 
Posts: 31
Joined: Thu May 25, 2017 7:23 pm
Model of CNC Machine: Shapeoko 3

Re: Help with Color Core Tooling/Toolpath

Postby LittleGreyMan » Tue May 22, 2018 11:43 am

John,

What are you trying to achieve? We have absolutely no information about your project.

Could you post a file with comments?
Best regards

LGM

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 690
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: Help with Color Core Tooling/Toolpath

Postby martin54 » Tue May 22, 2018 12:24 pm

As LGM has said we really don't know what you are trying to do, if you can't post the file for copyright reasons then a couple of screenshots would be the very helpful.
Depending on what it is you are trying to achieve there may be several different approaches to what you are doing. Don't think I have come across plastic specific V or engraving bits, endmills yes I have a selection myself but not v cutters :lol: :lol:

Just to add that it may be there is another substrate you could use for this project which we could suggest if we had more detail :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3810
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Help with Color Core Tooling/Toolpath

Postby johnelle » Tue May 22, 2018 2:14 pm

Nothing exciting here. I am really just trying to get the process down first. Colorcore is mostly used for lettering although you could do some symbol outlines, etc. I originally bought it to do trail maps for local hiking trails but that hasn't really materialized yet. Not unlike indoor nameplates, but this stuff is weatherproof, sun fade resistant, etc.

Attached is a pic of a first test cut which is just my daughter's first name and the official logo of her "uni." The results aren't terrible but like I said the bottom is rough. Also the serifs on smaller text really didn't turn out well.

...ok so I have tried to attach a photo but it just hangs in Chrome and Edge. This forum software is truly awful.

So in the picture you would see "Kate" in 1.5" height and "Binghamton University" in smaller (~ .75" / .5 ") text. Carving is fairly clean but some fuzzies on the top edge. Bottom of letters is relatively flat but would be better with a square end mill I think. Edges are pretty perpendicular to the surface. This was done with a standard 1/16 ball nose from Carbide (my machine supplier).

Here is the picture via the web https://photos.app.goo.gl/vxdOr85GrXfJrRWt1
johnelle
 
Posts: 31
Joined: Thu May 25, 2017 7:23 pm
Model of CNC Machine: Shapeoko 3

Re: Help with Color Core Tooling/Toolpath

Postby Bob Reda » Tue May 22, 2018 5:18 pm

colorcore does have the tendency to leave fuzzies which you have to clean out. Also there is a special bit for it, I got one but cant remeber where I got it.
Bob
Bob Reda
Vectric Wizard
 
Posts: 655
Joined: Wed Aug 16, 2006 7:34 pm
Location: Monessen, Pa
Model of CNC Machine: shopbot 48x48 upgraded prt

Re: Help with Color Core Tooling/Toolpath

Postby johnelle » Tue May 22, 2018 5:36 pm

So if you're doing color core:

1) What is the type of path that you are using for the letters and/or symbols?
2) What is the basic geometry of the bit you use (square? ball? V?)

Most of the plastic bits have a small number of flutes to carry away the big chips before they get hot and melt.
johnelle
 
Posts: 31
Joined: Thu May 25, 2017 7:23 pm
Model of CNC Machine: Shapeoko 3

Re: Help with Color Core Tooling/Toolpath

Postby adze_cnc » Tue May 22, 2018 6:16 pm

Every time I try to respond to this thread I get frustrated and delete it. Let's try again.

1) do not use a ball-end bit for this project. It is entirely unsuitable.

2) If you use v-bit with the v-carve/engrave toolpath you will get nice crisp inside corners but it the result may look odd because of the two-coloured material being exposed on the slope. Also you will need a square-end bit to clear the larger areas.

3) If you are wedded to the walls being perpendicular to the floor then use a pocket toolpath with possibly two sizes of square-end bits (large to clear out bulk; small to get into tight spaces). Inside corners will be round. You can't avoid it.

4) Read the help file regarding the various toolpaths. Search out the appropriate tutorial videos.

This really is a simple project that is being made overly difficult.
User avatar
adze_cnc
Vectric Apprentice
 
Posts: 405
Joined: Sat Jul 27, 2013 10:08 pm
Location: Vancouver, BC, Canada
Model of CNC Machine: AXYZ 4008

Re: Help with Color Core Tooling/Toolpath

Postby LittleGreyMan » Tue May 22, 2018 8:28 pm

I totally agree with Steven.

As the green material seems very thin, it may be worth giving a try at suggestion 2 (v-carve)
Best regards

LGM

W7 - Aspire 8.517
LittleGreyMan
Vectric Wizard
 
Posts: 690
Joined: Fri May 15, 2015 1:10 pm
Location: France
Model of CNC Machine: 3 axis small size machine

Re: Help with Color Core Tooling/Toolpath

Postby martin54 » Wed May 23, 2018 1:14 am

I normally use an engraving toolpath when doing this sort of work, if I am looking for a flat bottom to the text then I will increase the size of the flat on the engraving bit to help give a better finish, I have engraving bits not only with different angles but also with different sized flats on the bottom.
There are a number of different toolpath strategies that you could use, spend a bit of time going through the tutorials as Steven has suggested :lol: :lol:

As for your substrate try a google search for engraving laminates, Rowmark & Traffolyte are 2 brand names you can use to search, you will find that there is a wide range of engraving laminates available which will meet your requirements, generally plenty of suppliers which means you can shop around to get the best prices plus shipping may well be less :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3810
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Help with Color Core Tooling/Toolpath

Postby johnelle » Wed May 23, 2018 11:25 am

So setting aside the comment that I am over-complicating things my 2nd test cut shows just how hard it is to get a clean cut. This uses 3 very high quality bits, new or barely used running at the plastics company's recommended feed/speed:
https://photos.app.goo.gl/mBdVbovnWW8c8Hwy8

Line 1 was cut with a special O-flute plastics bit http://a.co/42VdORJ running at 60 ipm /15,000 per the recommendations. It is the cleanest but I was only able to use a font like arial because flat bottom bits can't really cut all the little serifs. Path was a pocket. Font size was .75 in. Bit was new.

Line 2 was cut with a 30 deg engraving v-bit https://www.ebay.com/p/30-Degree-Bits-for-Scoring-or-Engraving-Sharp-Point-Narrow-Tip-Kyocera-Tycom/1401705119?iid=151845694455&chn=ps using the recommended 150 ipm / 20,000 rpm. V-carve path. Font size .75 Had to actually make two passes because the 0.075 left some green behind so I did a 2nd pass at 0.1 Bit was new.

Line 3 was cut with a standard 60 deg v-bit http://a.co/e3RKnu2 using same feed/speed. Same font & size. Cut at 0.075. Ran the same path twice for clean-up. Bit had been used lightly.

My observation is that the top recommendation from the manufacturer performs the worst (30 & 60 vbits). My expensive Amana 1/16" O-flute probably did the best cut but is limited in detail. The small ball nose had the best performance overall--performing a pretty clean cut with a lot more small details. Next experiment may be with the same ball nose (Carbide #121 0.0312") with a pocket instead of a V-path (?) and perhaps a lower overstep (although it was at 19% already).
johnelle
 
Posts: 31
Joined: Thu May 25, 2017 7:23 pm
Model of CNC Machine: Shapeoko 3

Re: Help with Color Core Tooling/Toolpath

Postby Adrian » Wed May 23, 2018 11:52 am

I cut Rowmark engraving plastic all the time and just use standard two-flute 3.18mm down spiral cutters mostly. 2 inches per second at 12k rpm. When I use V-bits on it I use my 60 degree CMT laser point cutter.
User avatar
Adrian
Vectric Archimage
 
Posts: 8265
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: Help with Color Core Tooling/Toolpath

Postby martin54 » Thu May 24, 2018 2:33 am

Manufacturers recommended settings are only a guide & are generally meant for production type machines, the type of cut being made & the size will probably also be a factor I would think but couldn't say for sure, While the text you are cutting isn't tiny it is small enough to produce a lot of sudden jerky movements which can cause problems for a hobby machine such as yours because of it's lack of rigidity.
You would really be better doing some experimenting to find the speeds & feed rates that work best with your particular machine. you may well find that they are a lot slower than the manufacturers figures especially for text & graphics that are small :lol: :lol:

I don't think that particular Brand is available here in the UK but have machined a few other Brands like the Rowmark Adrian has mentioned, as well as sharp bits there are a few other things that need to be right for a successful result, your table needs to be completely flat & the spindle needs to be trammed to ensure it is square to the table along both Axis, hold down needs to be watched especially with the thinner materials as they tend to bow up in the centre when clamped around the edge, vacuum hold down is probably the best method but sticky tape methods work OK as well. Dust extraction has to be reasonable to prevent the cut chips welding themselves back on :lol: :lol:
My dust extraction isn't the best so when I am cutting materials like this I use an air line to blow the chips away, makes a bit of a mess but at least I get decent cuts :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 3810
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: Bob Jr, highpockets and 18 guests