Desktop CNC Router/Mill

[Rabs]

For thin sheets and small cutters I just use masking tape around the edge of the material to hold it down. This seems to work as well as anything.

[flubrush]

For thinner plastic sheet (Styrene, Plastikard, etc.,) I use double sided tape.   For very delicate work I get low-tack tape so that the work isn't damaged when being removed at the end.   The tape can be stuck directly onto the milling table,  but I prefer to use MDF on top of the table to protect it from over deep cuts,  and stick the tape to that.  I find that the best tool for removal is a loose Stanley blade which works well as a fairly gentle wedge under the edges to start lifting it off.   It also serves as a cutter for the tape,  and a scraper to remove bits of adhesive left behind.

 

I also bought some Seklema Multi-mat which worked very well

 

http://www.rowmark.com/seklema/seklema.asp

 

...but it is expensive - I think my square foot was around £60 from memory.   But it is not of even thickness and is intended to be used with engraving cutters which automatically adjust to variations in material thickness.     Some areas of my one foot square sheet were of the same thickness and could be selected for use,  but I moved on to using double sided tape on MDF which could give me about +/- 0.001" which was sufficient accuracy for the work I was doing.   IIRC,  I was getting about 0.015" variation across the sheet of Seklema which was too much of a variation.

 

Jim.

[Rabs]

Yep, I completely agree.  My post wasn't clear.  I also use a sacrificial layer of MDF on the bed and then stick the sheet to be milled on top of that.  With double sided tape you sometimes need to be careful if you are cutting through it with very small cutters at high PRMs because it can gum things up and make the cut messy or too hot.  If you're not going through then it's no problem.

[Etched Pixels]

Why MDF given the dust is quite carcinogenic ?

[flubrush]

Why MDF given the dust is quite carcinogenic ?

 It is flat and its thickness is quite constant so it is possible to set up a flat bed with the minimum of adjustment.  I've also used Contiboard which is also very good for flatness but have moved over to MDF since the Contiboard covering can tend to blunt cutters - even hard carbide ones.

 

I use double sided tape to hold the material on the MDF and the tape has a thickness which gives a little bit of wiggle room when trying to get the tool breaking through the material but not ploughing a furrow in the MDF.   With decent CNC equiment,  you should be able to set the tool height accurately so that you don't cut below the material surface,  but sometimes it is desirable to cut just below the bottom surface of the material if you want a clean cut.    In that case,  either the cutter end is in the double-sided tape layer (note warning about adhesive build up in previous message) or if a bit deeper,  actually starts cutting into the MDF.  But if it is only going into the MDF by a thou or less,  then there is little dust to worry about.   I think the main worry over MDF dust is when using DIY power tools where a large amount of dust can be created when cutting or planing.

 

I also use B&Q's "best" MDF which seems to be a bit softer than other types I've seen and doesn't seem to generate a lot of dust if I get a cutter going into it.   But like all things with dust,  you play it careful and don't ignore it if you start generating a bit.

 

Jim.

[Rabs]

Completely agree with the above MDF dust is mostly a concern for people using cnc routers to actually cut MDF and hence get lots of dust.  For a backing layer there's very little dust produced .  For PCBs I use a different sacrificial materialbecause it needs to be almost perfectly flat because the width of the isolation cut is set by the cut depth (angled cutter).  For general work MDF is ok.  I'm also about to 3D print a collar nozzle that will sit around the cutter and will connect to my vacuum cleaner - which will really reduce the dust!

[didcot]

Well finally had some time to set the machine up. Took a chance and put the basic software on my old xp laptop and it perfomed well. I did the usual man thing a speed read the manual. Attached are the results of my first effort. I literally just downloaded the image, created the code and of we went. I need to read the manual properly to get the different depths better defined. For a first effort Im pleased.

No prizes for guessing where my allegences lie.

 

didcot

[Rabs]

There's nothing better than when things just work.  And you couldn't have chosen a better first item to cut  - great result.  Whenever I buy or build a new bit of kit I usually do something boring like a box or a circle.

 

I'm really keen to evangelise some more high-tech modelling (see the threads in my signature).  To think that one of these machines, SLA 3D printers, CNC lathes and laser cutters are all within reach for home enthusiasts is amazing.  My local club could buy bit of kit like this for less than they spent on wires and connectors for their last layout - imagine what an impact that would have on the group's modelling.

[flubrush]

I'm not sure how good your CAM interface might be when attempting to generate GCode for more engineering or architectural subjects but you might want to look at Cut2d by Vectric to generate good 2.5D code.   I also note that it is recommended software on your machine's web site.  You can get a trial download which is limited in facilities,  but the trial version usually has more than enough available to give you a good idea of what it can do.

 

http://www.vectric.com/products/cut2d.html

 

 

Jim.

[raymw]

Hi Didcot,

 

If you want to play with text - 'trutype fonts' - completely free, and useful, try http://yertiz.com/cnc/text2.htm

 

There is loads of free, useful cnc/G-code, stuff out there - no need to buy any software -  spend your money on tooling 

 

Learn the basic G-code functions, and write the raw code in any text editor. That will be most likely the quickest way to profile simple shapes. Again, from my site, http://yertiz.com/cnc/gcode.htm may be useful.

 

The couple of plaques you machined, what was the material, and how long did it take?

 

Best wishes,

 

Ray

 

[flubrush]

Hi Didcot,

 

If you want to play with text - 'trutype fonts' - completely free, and useful, try http://yertiz.com/cnc/text2.htm

 

There is loads of free, useful cnc/G-code, stuff out there - no need to buy any software -  spend your money on tooling 

 

Learn the basic G-code functions, and write the raw code in any text editor. That will be most likely the quickest way to profile simple shapes. Again, from my site, http://yertiz.com/cnc/gcode.htm may be useful.

 

The couple of plaques you machined, what was the material, and how long did it take?

 

Best wishes,

 

Ray

 

Ray,

 

I don't want to start an argument here but I wouldn't underestimate the time and effort necessary to write good GCode if you don't want to ruin the tooling you've bought instead of software.   I write my own GCode - specifically to do 3D waterline machining of certain shapes and I don't want to spend a lot of money to buy (to me) expensive software to generate it.   But it has been a slightly rocky road to success over the past two or three years and I've learned a few hard lessons - with broken cutters.   For instance,  one problem is working out where the waste will be during and after the cutting and it can be quite easy to plough a cutter through a bit of waste with a rapid move command - and "ping".

 

For something like a panelled coach side with all the pockets and profile cuts,  I can generate the code in a minute or two in Cut2D.  Writing the same code by hand would take considerably longer and might be subject to a few bugs. :-)   So I consider £95 for Cut2D to be well worth the time saving.

 

In my case,  the hand coding of GCode came along when I couldn't get what I wanted from the CAM software I had and it was an interesting exercise to generate it.   For simple GCode operations,  I do it straight into Mach3.

 

Jim.

[Rabs]

Yes, and Mach 3 has a nice set of wizards built in which can do most simple things if you string a few together.

[didcot]

Hi Guys,

 

Thanks for the tips and to Ray & Jim for the links.

 

To answer Ray's question, it is plywood that I had lying around and took around 1 1/2 hours. It carves like a printer prints, left to right, index forward, right to left and so on. I had the feed down low as it was the first time in use. Doesnt seem to be the most efficient was to me. I have Vcarve to play with a well, but may well play with the G codes for simple outlines. Last time I used them was as an apprentice 20 something years ago.

 

didcot

[raymw]

Hi Didcot,

 

Thanks for replying, that's far quicker than what I used to get, back then. Many years ago, ( I've just realised it was about 17 years!) I messed around with the same idea, with my homebuilt machine. Using coloured Perspex, I could machine in an image, raster scanning, deeper cut for lighter shades, etc. Most impressive when held up to the light. A bit of a problem, I used cheap woodworking router machines as the spindle, to get the 20,000 rpm needed for the 0.5mm milling cutters (the milling cutters cost £27.00 each, the router £21.00). The jobs took about 14 hours for a 4inch square sheet. Often, the router would only last 6 hours, before the brushes wore out, or the fan disintegrated, then, of course the cutter broke too. Another problem, was if I showed the results to my friends in the machine tool business, they would never give them back. I have a few 'seconds' kicking around, not sure if I can take a photo, if I can find them. I could probably find the g-code easier, but I expect it would be a few megabytes, and no way would I write that by hand.

 

Best wishes,

 

Ray

[flubrush]

Hi Guys,

 

Thanks for the tips and to Ray & Jim for the links.

 

To answer Ray's question, it is plywood that I had lying around and took around 1 1/2 hours. It carves like a printer prints, left to right, index forward, right to left and so on. I had the feed down low as it was the first time in use. Doesnt seem to be the most efficient was to me. I have Vcarve to play with a well, but may well play with the G codes for simple outlines. Last time I used them was as an apprentice 20 something years ago.

 

didcot

 

Raster cutting is the normal way of cutting the job you did.  You could probably speed it up by using a larger diameter ball nose cutter and increase the percentage step over,  but the trade off is loosing detail in your finished piece.   1 1/2 hours isn't too bad for a CNC milling job - I've seen people quoting tens of hours for a job - like Ray has just done. :-)   Earlier on,  I said that I split my panelled coach side into three parts to get the milling time down to about three hours for each individual piece,  otherwise it would have been up to ten hours to cut a full side.

 

I've found that I can do a fair bit of juggling when cutting profiles and pockets in 2.5D to get optimum times and that can mean using as large a cutter diameter as I can when I can,  which means changing cutters during the job.  Mach3 allows me to estimate the time of a cut fairly accurately so it can mean a fair bit of iteration between Cut2D and Mach3 until the shortest time is found.

 

Another thing which might be slowing your raster cutting down is the acceleration of your Z axis.  If the acceleration is on the slow side,  then the X/Y travel will be slowed right down to allow the head to raise and lower during the cut.  I know that my KX1 doesn't have a wonderful Z acceleration either which is why I tend to prefer waterline cutting for any 3D work I do which takes the Z acceleration pretty well out of the equation.

 

But it's all good fun. :-)

 

Jim.

[black5f]

Hi

All looks very good and a warm welcome to the world of cnc. Cading stuff up can be very time consuming, but worth I think. There are an infinite number of things you can do now.

 

Check this out:

 

http://jasondorie.com/page_cnc.html

 

Half tone conversion of photographs, free, I tried it out. It works using a 60 engraver tool just drilling to different depths. I also tried it with a very cheap router bit, worked well.

 

 

Some contiboard I found on the garage floor, chip board with a paper coat, sprayed black.

 

Some one uploaded a 3d scan of a fossil so I used it for sons bedroom door.

 

Cut into a cutting board I got from Asda for £1.

 

I also did a mayan calender, lots of free dxfs or stls about.

 

As well as model stuff, just done 6 MK1 coach sides.

 

Please enjoy! Help is totally free.

 

Tom

 

 

[raymw]

^{One of the first things to do, is to check that the machine can mill a circle, and 'a square' square. I had backlash in one of my old retrofitted machines, so a year or so ago I finally got around to fitting  ball screws to the x and y axes. I've listed the simple test-piece g-code below (can't attach that type of file, afaik) which will verify if your machines can produce accurate circles and squares. You may need to change the speeds and tool size to suit your machine, and depth of cut and so on, but easy to do in notepad or most likely in your machining software. The fact that it should be climb milling should make no difference to light machining in plastic (I suggest you use Perspex, not mdf), but in steel on a lightweight machine, it is likely to give problems.}

 

^{If you don't get a circle  or the diagonals on the square recess are not equal - measure accurately with a vernier or digital calliper,, then you may be able to adjust the gibs or leadscrews if possible. I can now mill 'round things' - buffer heads, wheels, etc., from steel plate, good enough for 7mm.Now the fun will be fitting the ballscrew to the z-axis.}

 

^{It will pay you to make or buy maybe a couple of small toolmaker's vices - this from Axminster is OK    http://www.axminster.co.uk/axminster-sieg-x2-100mm-vice-prod577189/   ,   but replace the adjusting screw with one that is not made of cheese. One advantage of this type is that the moving jaw does not tend to 'lift up'.}

 

^{the code, fwiw, is below - cut and paste to a notepad file, labelled test.dnc, say.}

 

 

^{(Created 23:25:46 04/05/2012 from test.dxf)
(Post = ISO G-Code - Non Modal)
(Tool 13 6mm slot drill)
N1 G90
N2 T13 M06 S20000
N3 G00 X-0.2068 Y-22.8612 Z5.0000
N4 G00 X-0.2068 Y-22.8612 Z5.0000
N5 G01 X-0.2068 Y-22.8612 Z-2.0000 F50.00
N6 G01 X-22.8823 Y0.2943 Z-2.0000 F100.00
N7 G01 X0.1965 Y22.8946 Z-2.0000
N8 G01 X22.8720 Y-0.2608 Z-2.0000
N9 G01 X-0.2068 Y-22.8612 Z-2.0000
N10 G01 X-0.2068 Y-22.8612 Z-4.0000 F50.00
N11 G01 X-22.8823 Y0.2943 Z-4.0000 F100.00
N12 G01 X0.1965 Y22.8946 Z-4.0000
N13 G01 X22.8720 Y-0.2608 Z-4.0000
N14 G01 X-0.2068 Y-22.8612 Z-4.0000
N15 G00 X-0.2068 Y-22.8612 Z5.0000}

^{N16 G00 X33.1513 Y-0.1135 Z5.0000
N17 G00 X33.1513 Y-0.1135 Z5.0000
N18 G01 X33.1513 Y-0.1135 Z-2.0000 F50.00
N19 G02 X33.1513 Y-0.1135 I-33.0000 J0.0000 F100.00
N20 G01 X33.1513 Y-0.1135 Z-4.0000 F50.00
N21 G02 X33.1513 Y-0.1135 I-33.0000 J0.0000 F100.00
N22 G01 X33.1513 Y-0.1135 Z-6.0000 F50.00
N23 G02 X33.1513 Y-0.1135 I-33.0000 J0.0000 F100.00
N24 G01 X33.1513 Y-0.1135 Z-7.0000 F50.00
N25 G02 X33.1513 Y-0.1135 I-33.0000 J0.0000 F100.00
N26 G00 X33.1513 Y-0.1135 Z5.0000
N27 G00 X0 Y0
N28 M05
N29 M02}

 

N30 (how much do you remember, Didcot?)

 

I hope you can do a virtual run-through - see where/how to clamp it down

 

Best wishes,

 

Ray

 

PS, been a nightmare editing this - font sizing/spacing all over the place

 

[didcot]

Hi Ray,

 

That looks vaguely familiar. I remember the machine was a Bridgeport Interact, one of the first to have a graphics interface to show the tool path. We made a 2" thick sacrificial aluminium bed for it. It was in Apprentice Training after all and strange things used to happen!

 

As a general comment to everyone who as replied so far, thank you. This is a very friendly & helpful forum.

 

Right back to the Vcarve tutorials.

 

didcot

[Hawk]

Why MDF given the dust is quite carcinogenic ?

 

Do you have a source for that? As I use quite a lot of MDF, I checked the data sheets, but could find nothing to support that MDF dust is especially carcinogenic.

 

Quote from data sheet:

 

"MDF is largely composed of softwood bound together usually with a urea formaldehyde or melamine urea formaldehyde resin. When it is machined, very fine dust is produced. Just like “natural" wood dust this is a potentially hazardous substance and it must be controlled. For example wood dust can cause skin disorders and asthma. Hardwood dust in particular can, very rarely, cause nasal cancer - and as such is classified as a carcinogen in Control Of Substances Hazardous to Health (COSHH) Regulations. Theevidence that softwood dust can cause cancer is less conclusive. It is not classified

as a carcinogen in the UK. However, all wood can cause irritation and we draw your attention to the guidance given in HSE woodworking sheet no 30 Toxic woods."

 

What am I missing?

[-missy-]

Hello Hawk.

 

I would guess its the formaldehyde...

 

http://en.wikipedia.org/wiki/Formaldehyde

 

A known nasty.

 

Missy.

[Rabs]

And here for the chapter and verse:

http://www.hse.gov.uk/woodworking/faq-mdf.htm

[didcot]

Evening Chaps,

 

Its been a while and I have been busy. I initially had some problems with the machine not going back to zero properly and multi depth pockets misaligning. However after a few phone calls and emails came up with a plan. First fiddled with the play in the Y axis and that helped. Changing to a raster rather than profile in Vcarepro for pockets helped enormously. Changing the file output format to G code.tap was recommended. I don't know why but it worked.

 

So apart from welding plasticard with the cutter I have been working on Arley Station. I 3d modelled it and created the drawings. Barry Geens book on Arley has a 2mm scale drawing. I doubled it etc.

 

 

After sorting out the issues this is what I have come up with. I have even created a program to cut 45 degree angles, as I haven't go a cutter. Tip APT tools for good cutters.

 

 

I have started CNC cutting slates Flemish bond to go over the carcass. Its a bit tricky. Next time I will bond it to the base material, but lining up the brick courses it tricky.

 

cheers

 

Didcot

 

 

[malcolmy]

Wow that's brilliant! You don't fancy building a second one for me I suppose?!?

[mark84]

Hi Didcot,

the CNC machine you got seems great, it's exactly what I'm after I think. The station looks great...how are you getting on with the click n carve, would you give it a positive review?

Thanks, and happy new year!

Mark.

[flubrush]

Evening Chaps,

 

Its been a while and I have been busy. I initially had some problems with the machine not going back to zero properly and multi depth pockets misaligning. However after a few phone calls and emails came up with a plan. First fiddled with the play in the Y axis and that helped. Changing to a raster rather than profile in Vcarepro for pockets helped enormously. Changing the file output format to G code.tap was recommended. I don't know why but it worked.

 

So apart from welding plasticard with the cutter I have been working on Arley Station. I 3d modelled it and created the drawings. Barry Geens book on Arley has a 2mm scale drawing. I doubled it etc.

 

After sorting out the issues this is what I have come up with. I have even created a program to cut 45 degree angles, as I haven't go a cutter. Tip APT tools for good cutters.

 

I have started CNC cutting slates Flemish bond to go over the carcass. Its a bit tricky. Next time I will bond it to the base material, but lining up the brick courses it tricky.

 

That's looking good.  I'm glad to see I'm not the only one who has had to surmount problems of various kinds to get an end result. :-)

 

What size of cutter were you using for your windows?  I can hardly see any radius in the corners.

 

What programming did you do for 45 degree angles?    I haven't tried to do that yet but I would probably use a ball end mill and a bit of Gcode to produce the 45 degree angle,  although I would have to cut below the material bottom surface to work out the shape of the ball end.

 

I've also been looking at cutting planking in freight stock sides and have had some experiments with engraving cutters like these

 

http://www.ebay.co.uk/itm/cnc-router-engraver-engraving-tool-blade-cutter-bits-15-degrees-uk-/171044998042?pt=LH_DefaultDomain_3&hash=item27d3138b9a

 

I have had limited success so far and I suspect I am blunting the cutters - possibly by the way I set the height.  I set them to the top surface of the material and have been rolling a piece of rod of a known diameter under the tip until it just catches when lowering the head by small increments.  However,  I was using the 3mm shanks of broken carbide cutters to do this and I suspect that the very hard shanks are actually chipping the points.   I've been working on other things recently,  but should go back and do a bit more experimenting with some other method of tool height setting which won't damage the points of the cutters.   If I do get them working well,  I was also looking at engraving brick and stonework on styrene sheet for buildings.

 

Jim.