Printable View
Hi guys , Well ive finished the CNC build , Have almost masterd the software & cad drawings ,G,code etc etc. My question is about engraving my panels with my machine , I have found that I cannot get my lettering fine enough , could anyone give some advise on engraving white perspex, I do think i need to change the bit but is there any other tips you guys could give me Chhers all !! Riche......
Which tip are you using?
Thanks for the reply im using this bit the TV 2208 one
http://www.apworkshop.com.au/html_ro...ffb-vg225.html Cheers..
http://www.precisebits.com/products/...oreengrave.asp
These are the bits I use.
Regards......................Brian W.
Thanks for the reply Brian, Which of those bits would you use for the lettering on your panels, Do you buy them from US or can you buy them here in australia. also any tips on the process its self for perspex speed/depth/ etc etc Thanks again Rich..
Yes, I wanted to know what angle bit you are using as well....and since we are asking Brian lot's of questions, here's one more: What size font are you using?
Thanks,
BuddyM
Hello BuddyM
I have lately used a 0.4mm (or smaller) Endmill single flute (not V-cutter) with success.
Attached an image from SheetCam showing a part of the VOR panel in a B767.
The cutout of the letters is approx. 0,5mm wide and I'm cutting "Inside Contour".
I feel that the Endmill gives me better control of the width compared to the V-cutter.
When passing the panel paint, the width is final – that is not the case with the V-cutter.
I do two passes - one “Up cut” and one “Down Cut”.
Just some ideas which you could try…..
Forgot the Font question:
Mostly using "Futura Md BT" - Font 12.
http://www.hoddo.net/images/misc/engraving.jpg
Ok I mainly use the 60 degree ones. The 30 degree are very fine and if you do not have a very accurate spindle that does not have any runout, then you will easily break the tip off. As far as the depth goes you need to experiment with that to get the width you like the look of.
These bits are not available here as far as I know, so you will have to get them from the States. They are very fast on delivering orders.
The font I use are Stick40, and the size of course will vary according to the panel used.
Hope this helps..................Brian W.
Dear Richie,
first of all I would reccomend you use futura single line font. For engraving I'm using different tips with diiferent width to design how thik the line has to get. from 0,1mm t 1,5mm. thats the best way to have a good quality engraving. If you need single line futura just send me an email and I can send you an ABC in Futura or you use a program called text to dxf which includes a single line editor.
regards Mike
I just tell mine in this topic.
Engraving with the CNC is a long trial and error, and even an expert user sometimes ruin a piece for small forgotten details...
Anyway,
In my opinion only Vbits should be used to engrave the panels, other bits types might scratch or chop the paint. What angle mostly depends on the finishing type you want to have. Very sharper angled Vbits (10-25°) will give you a blind effect and harder to backlight, but more contrasted. 30-45° Vbits are the most used as a medium range. Wider Vbits (>60°) will tend to let perceive light floodings around the letters. Some people might like it some not.
All of those bits can be bought almost anywhere in the internet. Ebay has tons of sellers having them for cheap in all the flawours you might like. You can freely buy them in 10 packs but you won't use more then 1-2 to engrave panels as only paint has to be removed and is a very light job. Also consider the tip size. The best is always something in the 0.1-0.2mm range, that will give you enough freedom to engrave the most complex and even smallest chars. 0.5-1.0mm ones will be useful for bigger text and will speed up the engraving. Buy a set with various sizes if you can...
The most used font for panel engravings is the Futura Md BT (In truth the Futura DemiBold, but it's really hard to find and the Md BT is very close). This is not a personal choice but a rule of the MIL specs. Obviously the problem is that we don't have only to choose the right font but also the right depth of cut, the right bit and the right path allowance when cutting to acheive the best result.
My own is usually acheived by planning the text in the size I like in illustrator, make it outline, export to the CAM software (I use Artcam), make the engraving path with the 45° 0.2mm bit, 0.1mm depth and leave some small allowance to the paths. In this way I will be able to engrave a first time and check if I like it or bold a bit the chars by reducing the allowance and make a second run.
Usually two passes always give a cleaner result; the first removes the paint, the second clean and sharpen perimeters, so having 2 diffs paths with my method just speed up things and prevents from unwanted extrabold chars.
To end with, always check that your panel has the very same thickness in all of his parts. Irregular sheets are more usual in acrylic cast then polycarbonate (like perspex is) but check it anyway. Even 1/10th mm (0.004") difference matters. If a part is thicker then other you will finish for sure by having a very bad engraving in the part where the perspex is taller, because the bit will dig too much into the plastic.
Thanks all so much for your replys , I will do some shaves & post some pics soon , One more thing just about the spped of the router is fast or slow better, would it help to try & cool the bit as it shaves the paint cheers all!!;)
yes, thanks everyone for the terrific info. I will post some pics when I get respectable results, so far less than optimal.
BuddyM
Ok here we Go, Here is a few pics of my first cut/shave , I do need to get a finer bit but I am quite happy with this , must admit there is a great sense of a achivement when it all comes together , I started building my CNC machine around 6 months ago & have learnt so much since, Thanks again for all the help & advise of all here, Cheers !!;)
Well done. I know exactly what you are going through, having designed and built my own CNC. You can't beat it !! The finer bit will help a lot, as I was using exactly the same bit you are using at the start. One thing that had me fooled to begin with was engraving first, then cutting out the outer edge. I then put a rail with a right angle onto the top table ( I also put a 20 mm. MDF piece on top of the CNC table to save it from holes ! ) so that you can then cut out the whole panel, then sand and paint it and then return it to the same place to do the engraving. Makes things a lot easier and neater.
Regards....................Brian W.
fantastic looking panel, great job! What type of procedure do you use to paint them?
BuddyM
Funny you ask, The paint is just a spay primer that they sell just down the road from me ,only $2.50 AU a can from a car shop, I really dont know how much diffrent it is from the real boeing 737 color, Dont think it is to far off.(other primers i have seen seem to light) That panel in the pics was my first, & i gave it 3 coats before engraving also did leave for about 24hrs to dry not real sure if thats nessasary though, thanks again to all for the tips , I will now start to crack on with the pit, Thats been sitting dormant for the last few months Check out the pics http://www.mycockpit.org/photopost/m...3830&protype=1 Cheers guys!!! :p
MMMM not really sure how i would build my own CNC but was wanting to make some panels but also not sure on what the panel is made out of.... is it a metal sheet? also could i buy a CNC or take it some where to get my panels made?
I built my machine from scratch, using a 14-page plan set I bought off ebay. It wasn't difficult, and it is very accurate. I built it just to cut sim parts, but have found several other uses.
My machine uses friction bearings and 20 tpi screws, so it runs very slowly which is a problem for cutting plastic. I am building a new one from a kit right now, and it has real linear bearings and real drive screws. It will run much faster, so plastic wont be as much of a problem.
there are lot's of folks here that might cut panels for ya, all of mine are plastic. When I get the new machine running and learn how to engrave the lettering and legends properly I would be happy to make a few for folks....
Buddy
NICE thanks!!!!! Also i found another need for a CNC to helps make my Circuit boardsQuote:
Originally Posted by Buddym
NICE thanks.... I also noticed that i could also use one to make my circuit boards
Ok so I know now which type of bits to use for engraving. (nice Thankyou) My next question is which is the best bit to use for cutting out the holes for buttons, switches,Displays, etc etc? & whats the process for holes ,should or can you cut with one pass or 2/3??? If anyone interested this is the site i followed for my CNC build http://buildyourcnc.com/latest.aspx Thanks all .. Riche
Here are the bits I bought from Precise bits (www.precisebits.com) to make up a nice all around kit based on discussions I had with Vince (vcimmino):
4 - MM208-0313-013F 0.8mm PreciseBit
4 - MM208-0394-020F 1mm PreciseBit
3 - MM208-1181-050F 3mm Bit
1 - MM208-1250-125FL 3mm DeepReach
1 - EM2E8-1250-30V 30°
1 - EM2E8-0625-45VW 45°
1 - EM2E8-0625-60V 60°
1 - EM2E8-0625-90V 90°
1 - MM208-0625-020B BallNose
10 - DC208-M080-040D Drill Bit 0.8mm
10 - DC208-M100-040D Drill Bit 1mm
On smaller bits <1mm you may break easier hence the larger quantities. The MM208 bits are for cutting, the EM2E8s are for engraving, and the DC208s are for PCB drilling.
Hope this helps,
Scott
Thanks so much for reply , gunna place my order now, I will need a collet for these bits im guessing my router takes 1/4 inch shank , would someone point me at the correct collet i would need for those bits from http://www.precisebits.com/search_re...I1.x=10&I1.y=9 wouldnt ask if i could get them here in australia cheers again guys..;)
Rotozip makes a collet adapter to go from 1/4" to 1/8". It uses a set screw to hold the bit in the collet adapter. Actaully works out nice. Very cheap though and you may find a little runout on these. There are also extremely expensive collet adapters out there as well. The Rotozip one has worked fine for me.
http://www.plumbersurplus.com/Prod/R...=2&cvsfp=95452
I bought a collet adapter for 1/4 to 1/8 at Sears. Works great
BuddyM
Hey guys , heres a small update on my progress,( pic attached) Im still experimenting but The panels are getting better, I still havnt purchased the right endmills yet ( moneys bit tight) But im sure the right ends will give me what im looking for, Very happy with my machine dosent seem to have much runout atall which helps alot i think. Im really enjoying the Whole CNC process, its bit like another hobby to add to my other 4 or so i have (not enough time in the day!!) Anyway thanks to all who gave me great advice about this subject Cheers Guys!! Riche...
Nice job Rich, :) :) :) Fantastic to be able to build your own panels :) :)
Matt Olieman
Hi Guys, Just curious how other cnc users clamp there work to the table for cutting/Engraving, I have Drilled hundreds of holes into my table using a jig, I then use the plastic shelf supports you would use in kitchen units etc etc, To clamp between the piece & the table, What i have noticed is that on some of my perspex panels, they are slightly rasied in the centre from the table 0.5mm roughly, While the edges are tight to the table. This is fine When cutting the holes in the panels , But when it comes to engraving the letters arent consistant thoughout , Any Thoughts on how to get my work perfectly flat. Cheers ALL.. Riche...:)
Dont Laugh as i cant remember where i read it, but some guys have succesfully used small dabs of superglue to hold thin material down and were able to prise the part up after machining without damage to the part ( will try to find the source of that info but it was legit ) also Double side tape strategically placed would, again allow for machining and removal after ... just a thought but as you find out there's "a load of ways to skin a cat" as the saying goes ( ok not a animal friendly quote i know but you get the gist LOL:-0 ) Cheers..
Hello ba543
A vacuum table would maybe be the best, but then more investment needs to be done. So far, at least I have been able to mill quite successful – even engraving. I have a few different methods to fasten depending on what to do and there is certainly other ways of doing this depending on your table facilities.
- Most normal is like your doing – clamping down to a flattened table (or scrap-board) along the edges of your material. This for taking out holes and pockets and some time the cut-out of the panel
- For front milling (pockets. holes & engraving). Those panels which have mounting holes, (most have - like the MCP have 8 holes) I first mill these holes to 2,5mm while clamped described above and down in the scrap-board (>10mm extra). Make the panel holes to 3mm afterwards. Then I thread the holes in the scrap-board for 3mm bolts and use this is as the only clamping – more than strong enough – even for the final cut-out. Be sure to set the “rapid clearance” well above the bolts. If you take care of your Zero position for the specific panel you have now a nice jig which you can use several times – in and out with the panels for inspection and e.g. painting.
- If the above is not possible you will need some double-sided tape (not tried), but then you backside need to be more or less flat. In case of engraving you don't need the stronges mounting - just enough to keep to the position under light forces from the carving tool.
For all this you need an absolutely clean and flat table/scrap-board.
- The last one is for PCB production – just ordinary masking tape along the edges.
Just an example:
http://www.hoddo.net/images/cockpit/glare/MCP-Front-back-2.jpg
Happy milling
Does anybody have any ideas on how i can go about making a cheap CNC machine here at the house?
I built a cnc machine for about $650 not including software. I researched it a long time before deciding what to build. It is built from high density plastic using plans from the internet. It is very slow due to the power supply and controller running the stepper motors at only 12 volts, and using friction bearings made of Delrin instead of linear bearings. It works quite well, but not on Plexiglass. The slow feedrate causes the plexi to melt onto the bit and breaks the bit. (The VERY expensive bit, $35 each delivered.)
I bought a Probotix V90 Fireball kit about a month ago and have been cutting with it since then. It is 10+ times faster that my DIY machine and is very precise. I have cut 1/4" polycarb plastic at 90 inches per minute, which should be fast enough to try plexi, just working up my nerve to possibly break another bit.... The V90 is about $1000 delivered, not counting the router and software. It assembles in about 2.5 hours
Learning CAD/CAM has been the challenge for me, I only recently started getting acceptable results when engraving. The right bit and font make all the difference. If I was building the machine just for sim panels I might just buy commercial panels, since by the time you add up the machine, bits, software, and ruined material, it is probably just as expensive as buying panel kits, if not more so. I love to tinker and build different things so building a CNC machine seemed like fun. It was also very time consuming and frustrating at times (still is). Also very rewarding when you get good results.
BuddyM
In the hands of a skilled CAD/CAM/CNC operator I have no doubt that the V90 is capable of doing fantastic work. I am still learning CAD/CAM so my results are not anything close to what you will from Phil and others here.
BuddyM, your plexiglass problem might be because you are using Extruded Plexiglass. You will need to use Cast Plexiglass to stop it from melting.
Hope this helps. Tom.
Thanks Tom,
I had heard that over on the CNC Zone forums as well, but have not picked up any cast plexi to work on. If I can get past that, then making nice backlit panels with engraving is now within my reach.
BuddyM
Tom is absolutly right in what he says, for light plates avoid extruded acrylic at all costs, cast is always better, its easy to machine and 9 times out of 10 you can get away without annealing.
I dont use CNC for my panels, i dont even own one (yet;)) but one thing i would say is be very careful when machining, you need to keep the router bit as cold as possable, probably get away with just using an air blower but water is always better, the reason is that if the router bit is too hot you induce thermal stress into the acrylic, basically the very edge of the freshly cut face has been hardened by excessive heat where as the rest of the acrylic is soft in comparison, if you look carefully sometimes you can see it, this becomes a problem when painting it because the chemicals in the paint softens the acrylic and cause microscopic cracks to form, you will not notice it a first but several months later you will spot light bleed through along the edges, ive seen panels from many vendors that suffer from this problem, using cast avoids this issue 90% of the time, if you are unsure cut a test panel and soak it for 48 hours in isopropanol, that will tell you if you will have problems, but if you kep the job cool whilst cutting you will be ok.
As for mounting panels for engraving i have a simple solution, the engraving is usually the last process before installing the hardware, some of my stuff requires cutting via laser after its been painted and engraved, basically I made a Dzus rail bed that accepts the pedestal size panels, assemble the light plate to its back plate then fit onto the Dzus rail, I always use the top left Dzus as a reference point for the art work/ cut work
Phil, thanks for all the info, I have heard great things about your panels, so the info carries extra value. I will post some photos of my work when I get some cast plexi. I have also cut some panels from plain old polycarb, both black and grey, and then smeared the engraving with bright white enamel paint. I did flaps and speed brake panels like this and they came out great.
BuddyM
Excellent information Phil. Giving away all your secrets :) :) :)
Thanks for the info.
Matt Olieman
Yes, Phil's panel are great. I wish I could do the same......
My wishes for next Christmas is a 1 KW laser "burning" out the whole cockpit in one single run from of a huge block of acrylic...:D finished in a couple of seconds.
that would be nice..... I don't think my Santa has the budget for that!
BuddyM
Hi all, I have been trying to hunt down a supplier of the fine mill ends here in australia & i have found one here is the link http://www.mcjing.com.au/categorybro...?categoryid=27 I was able to visit the shop as it is only 30 mins from where i live. You will notice the fine bits arent advetized on the website but they have the biggest collection of mills,drills,collets,etc etc,I bought some 0.45mm bits for engraving at $4.00 per piece. The lady in the shop is very switched on she will know what you are talking about as long as you ask for the correct bit you are looking for. anyway im sure this will help a few of you here in oz & save you $30+ on shipping , Doesnt feel as bad when you break a $4.00 bit. While expirementing with these bits i found 0.45mm gives me nice lettering not to wide you do have to be careful with the depth being so thin they will snap easy, also your work must be totally flat to the table ,which i had problems with earlier, then a simple soulution of some wide double sided tape, carefully stuck to the back of the panel, plus my normal fixtures on the side gave me good results. will post pics of these shortly. This is still all new to me ,But slowly getting the results im looking for.As said by others the cnc process can be very rewarding:o & disapointing:( , its fine tuning everything together carefully. I have varible speeds on my router, & have found depending on the bit being used to cut , slow speeds & feed have worked for me. (expirement). Is there a way of knowing if the plexiglass/perspex is cast or Extruded, Im using an old frosted sighn that used to hang out side a shop that was light up???? seems to work, Anyway will report back soon with some pics Cheers all .. Riche..
It's funny to see here how several total different approaches can lead to great results.
As mentioned here before: patience, experience are far more important then some technical things.
Seeing this thread rather late will write some of my experience here.
Flatten underground. Engrave word by word or circle by circle and every time adjust the Z-height (because of the imperfectness of the material etc.). I make 3 or 4 rounds every time 0.05 mm deeper (depends on the thickness of the paint of course). Try to only remove the paint. When satisfied I stop the proces. With my finger I rub the the new engraving. The burrs drop in de new engraving but are now removed very well. After that one time more engraving removes everything and the white is really white. Try to fix the panel at the upper side. is more equal than from below. Mirror by making at the back, holes of the thickness of the mill, so in fact drill not mill (even if the holes must be widened later (e.g. for rotaries 6 mm). Using these small holes which fit narrow around the mill it's more easy to center the front side (the mill exactly fits in the hole !). I use (really !) ball nose mills .. from the dentist (0.3 mm). The reason is that they nearly make a flat path (in contrary to the V cutters). Flat would even better i.mo. but could'nt find flat end mills of 0.3 mm. The cut only removes the paint en does not go very deep in the acrylic material. This "flat bottom of the canal" is more Boeing like (to me). See also in fact the same comment of Per-Erik (Perik) in this thread. Less (!) translucent white acrylic gives a nicer appearence of the white when not backlighted. Never use backlight right behind engravings, always take as much distance as possible (diffuses the light too). Round all the edges (realistic and better for holding the paint).
Hessel
http://www.mycockpit.org/forums/atta...0&d=1246474842