PDA

View Full Version : First engraving test :)



Davek0974
19-04-2016, 07:41 PM
Had a play with engraving tonight, most impressed :) The more i mess about with my machine the more i like it.

No idea of the proper way to do it so i used SheetCams' built in text tool and used a lump of scrap ally.

Tool was a 1/8" 90 degree carbide bit that was given to me a while back, i guessed 24,000 rpm, 165mm/min feed and 65mm/min ramp in.

DOC was 0.2mm in two passes of 0.1mm having no idea of correct depths.

Result looked really nice - 96mm long

18231

Close-up...

18232

So, what is the 'correct' set up for this as i can see uses here ;)
Are there better tools?
Better feed-rates?
A correct DOC?

Fun stuff ;)

cropwell
19-04-2016, 08:34 PM
Hi Dave,

Engraving looks good !

I find the problem is usually getting the material flat enough to the X-Y plane to get an even DOC. Taping down to a sacrificial MDF surface which I have skimmed generally works. I use chisel engraving bits with a 0.2 mm flat on the end.
1823518236
Here's a couple of examples, both are low res photos. The first was done with the chisel point engraver, it is 60x20 on .5mm brass with .1 DoC. The second is done on fibreglass PCB using a 1mm two flute cutter to cut through the copper. It looks good with backlighting but the furnace is never switched off long enough to put that in ! I got the picture by capturing a webcam image, so that too is low res.

Davek0974
19-04-2016, 08:38 PM
Nice, I cant be too far off then, what sort of feed rates do you use?

I have a pack 10 30 degree tapered bits with 0.1mm tips - too fine??

With a DOC of 0.1mm do you do that in one hit?

cropwell
19-04-2016, 10:28 PM
Nice, I cant be too far off then, what sort of feed rates do you use?

I have a pack 10 30 degree tapered bits with 0.1mm tips - too fine??

With a DOC of 0.1mm do you do that in one hit?


a. 2540 mm/min
b. depends on what you are doing
c. yes

Cheers,
Rob

Davek0974
19-04-2016, 10:38 PM
Guess i was running a little slow then at 165mm/min ;)

Boyan Silyavski
20-04-2016, 12:48 AM
Many people really miss the main point. All really depends on the stick out of the tool. The shorter the stickout the faster you could go even with 1/8" tool. i would greatly recommend HSMAdviser. Not only its a great program, but most of all opens your eyes about when you change this and that how to achieve the even most important main point of all this- better material removal rate :single_eye:. At the end id does not matter what you do and how you do it. The removal rate matters.

Davek0974
20-04-2016, 08:17 AM
Thanks Boyan, I have subscribed to HSMAdvisor but engraving seemed to be throwing up some very odd figures.

John S
20-04-2016, 11:32 AM
Dave,
I think also you have backlash issues with the machine.

In the close up you have backlash marks at the top of the o and c and bottom of the d, u and s

I would worry more over this than speeds and feeds.

Davek0974
20-04-2016, 11:47 AM
I'm not convinced, it looks more like poor path generation - the letters are made up of lots of short straight lines and not arcs, I'm not sure the built-in SheetCam fonts are much good for this type of work.

If it is backlash then it is what it is and not much can be done about that - it's all new and I'm not about to refit it :). It does not affect normal milling work so i'm not 100% concerned about it TBH, these letters are pretty small.

Will need to try text generated in another package before condemning it I think;)

John S
20-04-2016, 12:01 PM
Are you using Mach3 ? if so I can send you a v-carve file for one of the fine engraving tips you have as a test.

Davek0974
20-04-2016, 12:04 PM
Yes, Mach3 and 2010 screen-set.

A file would be good, thanks

John S
20-04-2016, 12:18 PM
OK, I'll sort you something out tonight unless you want something specific like text and size.
Screen set will not have anything to do with it, we use a custom one anyway with everything we need on one screen.

Email me details of the cutters, included angle and tip flat as it alters the appearance on V carve files if not matching. When they match you get a sharp corner to the text, if incorrect you get an indented radii in each corner.

john [at] stevenson-engineers.co.uk

Davek0974
20-04-2016, 01:00 PM
Just had a look at the code and it is indeed made up of thousands of lines of straight cuts.

I did a quick file in Illustrator then imported that into sheet-cam and with the same tool it now creates I/J arcs so in theory at least that file should cut a whole lot smoother I think.

Boyan Silyavski
20-04-2016, 05:22 PM
Yes, many times this is the reason, the line thing instead of curves. I always magnify before generating path, to make sure all is smooth .

I would say also for fine engraving to have the Z0 using probing with the V bit itself is the best method. That, and knowing the exact tip size.

Davek0974
20-04-2016, 07:05 PM
Yes, i always probe with the actual tool.

I tried cutting the Illustrator file tonight, yes it cut far smoother but it was generated as two paths which gave me a letter with an inverted V in the middle ;)

A settings issue, wrong font, wrong code generator, other problem?

Lots to learn here...

Boyan Silyavski
20-04-2016, 08:40 PM
I think Vectric Aspire / V carve/ beats all when we are speaking about signs and engraving

Davek0974
20-04-2016, 08:41 PM
Blooming expensive though :(

Boyan Silyavski
20-04-2016, 08:58 PM
what are you using now?

Davek0974
20-04-2016, 09:07 PM
My CNC world consists of CAD - either Deltacad or Illustrator, CAM - SheetCam, CNC - Mach3

Apart from some free programs that i downloaded for messing about with that's about it.

Vectric V-Carve was about 400 I think - a lot of cash for something that is unlikely to bring cash in via sales I think.

Clive S
20-04-2016, 09:15 PM
My CNC world consists of CAD - either Deltacad or Illustrator, CAM - SheetCam, CNC - Mach3

Apart from some free programs that i downloaded for messing about with that's about it.

Vectric V-Carve was about 400 I think - a lot of cash for something that is unlikely to bring cash in via sales I think.Yes but you can use it to import dxf files and cam them with it.

Davek0974
23-04-2016, 05:00 PM
Following assistance from John S (thanks John) I have done some more engraving, this time using code generated in V-Carve and using my 3mm 30deg 0.2mm carbide cutters, the results were mind-blowing - razor sharp lettering, no burrs on the edges, could not be better and proves the machine is totally capable of detail work...

18278

It was not without issue though as I am 99% certain that the first plunge took the ridiculously fine tip off the tool as the first pass at Z-0.25 was air-cutting, pretty certain i could see the tip come off as i was watching pretty closely. The cuts above were done after this though so the results didn't suffer, maybe too fast a plunge rate?

So, in the last few days I now have a working setup of Vectric, nice software it seems, still reading the manual ;) It is intuitive though and have got a test text file I was messing with, setup some tools, hopefully using the same settings extracted from Johns' file but this time using a 3mm 60deg carbide bit as this angle seems the most common?

The results were nowhere near as good and I was bit disappointed with them - there are burrs on the edges and the cuts are generally crap under a magnifying glass looking like they were hacked out with a machete ;)

18279

So, obviously lots to learn here, any pointers???

Boyan Silyavski
23-04-2016, 05:56 PM
Following assistance from John S (thanks John) I have done some more engraving, this time using code generated in V-Carve and using my 3mm 30deg 0.2mm carbide cutters, the results were mind-blowing - razor sharp lettering, no burrs on the edges, could not be better and proves the machine is totally capable of detail work...

18278

It was not without issue though as I am 99% certain that the first plunge took the ridiculously fine tip off the tool as the first pass at Z-0.25 was air-cutting, pretty certain i could see the tip come off as i was watching pretty closely. The cuts above were done after this though so the results didn't suffer, maybe too fast a plunge rate?




Great!

Its a common problem- about the tip i mean. I am extremely conservative with the plunge rate of V cutters, even in wood.

Davek0974
24-04-2016, 12:14 PM
Bit better today, dropped the feedrate to 500 and plunge to 150, this was the same file - new one on top, yesterdays' one below - a much better result but still a tiny burr on a couple of the verticals.

18280

15mm high 'T' this time with a flat-plane limit set of 2mm so it bottoms out. Came out very nicely i think, picture does not do it justice, iPhones suck at macro work ;)

18281

Boyan Silyavski
24-04-2016, 01:28 PM
http://www.mycncuk.com/attachment.php?attachmentid=18281&d=1461492653&thumb=1


That T is great! i forgot, do you use mist cooling?

Davek0974
24-04-2016, 03:35 PM
Yep, its a home-build minimal quantity coolant system - I'm running on paraffin/oil at about 95% paraffin, I put 500ml in the tank when i built it and its only gone down about 200ml so far and i've done quite a lot of cutting and messing about ;)

You can just about see the film on the metal when cutting, I turn it up a little for deep cuts.