CNC by trial and error!

[Warhog]

For the price I couldn't help but buy one of these cheap chinese CNC's.

 

And they look really nice as well.

 

I have been trying to steer people away from these machines only because of the limitations they have related to cockpit building. Most of us would use CNC to make virtually all the parts one would need in a cockpit. That said, if all you need to do is engrave plastic you should be OK once everything has been tweaked to its max. As soon as you start to cut into anything heavier your going to get flex and there goes the accuracy.

 

To help maximize it's potential you should chuck your cutters so very little is showing out of the collet (z axis - Spindle flex).

 

Based on the v-bits I suggested I would make the cut depth for engraving plastic no more that 0.003".

 

Set your spindle speed close to max. If you see any melting... tune it down. I don't know what your spindle speeds are . If they are variable, you need to experiment with that. For engraving, faster spindle speed is generally better.

 

Feedrate for plastic is 30in/min. If you get any distortions in the letters, set it lower.

 

Use the double sided tape I suggested. Cover the entire back side. Clamps should not be necessary if you do that. Besides, clamps tend to cause distortion and create an uneven surface... very bad. Make sure that there is tape on both sides of what would be to outline cut for a panel. That edge is especially prone to being lifted when using an endmill to cut it. All edges are prone to this. Its just the nature of the endmill to lift material as it cuts it. If you don't ensure good coverage of the tape you will have your edges looking pretty bad. Also clean you table with isopropyl alcohol or acetone (assuming no plastic parts on the machine or they melt). That will ensure the tape has a good surface to adhere too.

 

For all other cutting I would use HSS or solid carbide 2 flute, 0.0625" (1/16") dia. end mills. If you need to pocket large areas go to 1/8" or if really large... can you machine handle 3/8" dia?

 

As you are new to CNC, I would strongly recommend you look into buying CamBam. It is so easy to setup your g-code. All you do is import your dxf file and set your type of cut, type of cutters and a few other variables and then hit the "make G-Code" button. It calculates all of your offsets for you, toolpaths etc. It is the most idiot proof package I have seen to date...why do you think I use it?:music_whistling: And it only costs $150.00. I think HSM might be a bit overkill as all you are cutting is 2 1/2 D parts, not 3D. CamBam can also be use in 2 different scenario's...basic and advanced and that can be set on the fly so if you need something special for one cut you can switch to advanced and then switch back for the basic. And one more point, you can draw your panels in it as well if you wanted to do that. It has good control over text and that will be a priority.

 

Thats all I can think of for now. I'll add to it as I think of anything else that may be important.

[ClayM]

Thanks for the advice Warhog. I'm going to buy CamBam. I really like the fact you can draw parts directly in the program. Sounds great.

 

 

 

First successful test cut. I initially made mistakes regarding pocketing or slotting but I am very happy with the outcome of the yaw trim! I know these chinese cnc's are pretty weak but if I can cut all the panels with similar quality to this I will be happy!

 

Gotta go download CamBam

 

 

Clay

[Deadman]

If I may suggest you make a circle for the arrow on the knob to be back lit.

Then make a small indent at the 6 o'clock position in the face of the light panel this with give you a center detente if you drill a hole and stick a small spring and a ball bearing in the whole in the knob corresponding to the dent in the panel.

[Warhog]

Thanks for the advice Warhog. I'm going to buy CamBam. I really like the fact you can draw parts directly in the program. Sounds great.

 

 

[ATTACH]121077[/ATTACH]

 

First successful test cut. I initially made mistakes regarding pocketing or slotting but I am very happy with the outcome of the yaw trim! I know these chinese cnc's are pretty weak but if I can cut all the panels with similar quality to this I will be happy!

 

Gotta go download CamBam

 

 

Clay

 

It looks like you have it set up spot on. Just the line work needs some attention. When I create lines, I start by drawing the line and then I offset it 0.015" to each side and finally close the ends. That gives me a closed poly line 0.03" wide. I use the pocket function to cut it which ensures there is nothing left inside it.

 

As DM mentioned, you can pocket out the area under the knobs for backlighting. Use the same technique except switch to a 1/8" endmill.

 

Mods and things to think about.

1. Use a small shop vac with a small diameter hose and attach it to the spindle bracket. A small pencil type attachment or a shoe/brush attachment will remove swarf as its produced keeping you table and machine clean. There are lots of examples on the net to look at.

2. When cutting acrylic...If you have a compressor, attach a fitting to blow a steady stream of air onto the cutting tool. Don't need a lot of pressure. This helps keep everything cool and the acrylic won't melt as fast.

3. Setting zero on your Z axis... Keep your jog rate set to 0.001". Use alt -pg dn to get your cutting tool close to the work piece surface. Then turn spindle on, jog down at 0.001" increments until you either hear contact with work piece or see it. Back off 0.001" and then set zero on you DRO and do a recalc. Your z axis starting point will always be perfect.

4. Keep a fine hair brush 1" wide to move swarf from cutting tip/workpiece when cutting to maintain visual.

5. Even though CNC is an automated process, NEVER leave your machine. If you do it will get mad and run itself into something just because your not there to hit the E Stop button. Happens every time.

 

For the time being, hold off cutting anything harder than the engraving plastic. Use it to get comfortable with Mach3 and the machine in general. It's easy to make mistakes at this point in the learning curve and it's always better to have soft material in place when you :doh: Now you may be tempted cut some aluminum. Just a little piece he says...don't. Stick with less damaging materials for now.

 

That's about it for now Clay. Keep posting like this and I'll add comments as you move forward. Beginners can use this thread to get them started.:)

 

John

[Warhog]

DM.....I had no idea there was a decent for the yaw trim knob. Excellent. I shall add that feature. I mean it makes perfect sense to have neutral trim snap into place.

 

Thanks Ky.:thumbup:

[LynxDK]

Wouldnt that Decent be obtainable from a Balance Potentiometer?

[ClayM]

DM

 

Thanks for tip. Hopefully one day I can have more accurate knobs. If I recall correctly you were producing these at one point. Is that still the case? Also is it just me or maybe I'm using the wrong knobs but are the shafts on common pots too long for our applications?

 

Warhog

 

I have to start taking notes to remember all this! I agree with never leaving cnc running unattended. I have had to use E-Stop a few times. What I have found with this machine is that i can set cutter depth in the collet at a point where at max -z it just clears the machine table. I accidently set wrong Z home once and the first thing that happened when i ran the program was plunging all the way through plastic and deep into my 3/4 mdf spacer. Luckily i had my finger on the e-stop and was able to stop it before it made any x/y movement. Engraving bits can drill through mdf like its butter!

 

So the reason I started actually building the pit was that I had Dimebugs plans, Gadrocs Helios and what finally convinced me was reactorones panels! Following the .375" rule some of my current panels dont make sense. I've put some of Lars' panels through inventor and there is some discrepencies but they do look really good! I'd really like to just take reactorones panels as templates and go with it. Starting from scratch would take me years ( or never) and I would still be guessing at most dimensions. For example Lars' UHF looks fantastic!

 

Comments please! I need somewhere to start. Otherwise I'm going to get my calipers out and copy reactorones panels. They have served me well for over 2 (maybe 3) years.

 

I'm attaching pre-cnc pit pic now. Lets see were it ends up! (sorry missing main monitor. its hooked up to mach3 on another computer. guess i need another one)

 

 

 

Thanks Guys

 

Clay

[Deadman]

I have made high quality replica knobs in the past but do to the lack of orders I have not made a resent run of knobs. http://forums.eagle.ru/showthread.php?p=2427515#post2427515

 

I have no idea what length of shaft your dealing with.

 

Check my thread if you want a replica you will find some interesting things My cockpit plans are very close to being finished I am reworking left and right console kits a change of thickness of sheet metal has made a complete rebuild necessary but will result in savings. Back plates for the control panels and the for the main instrument panel will be available for purchase as well.

Edited September 4, 2015 by Deadman

[ClayM]

Status update

 

I have been experimenting with CamBam and have some mixed results. From previous posts ( i think a couple of pages back ) you can see I had pretty good results using HSM. Heres what i am getting with CamBam

 

 

Setup as a .010" cutter. Using engraving routine. I'm a little confused why it would cut text to wide but still leave material in the middle.

 

Never mind

 

I just realized I should have used pocket instead. Is it safe to assume that engrave cuts on the center of the line instead of offsetting for tool radius like pocketing does?

 

On another subject

 

I managed to level a piece of mdf to use as a base to attach my work to. Using a 1/16" cutter to cut a 10" by 12" area was slow going. I would like to paint or stain or something the mdf to prevent the double sided tape from peeling the mdf. Any suggestions? I'm still a little hesistant to attach the work to the table.

 

ClayM

[LynxDK]

I would still suggest that you lvl off a piece of acrylic insted of MDF.

All your problems with paint, and things not sticking goes away, plus you can clean it easy with mineral spirits when There is still tape residue left.

[ClayM]

I am going to get rid of MDF soon! I was just being lazy and using what I had kicking around. As my supplies keep building up I will make everything a little more "proper". I have received my order of cutters and the rowmark I ordered finally showed up. So things are progressing. I will see I they also have a crop that would work for the new base so I dont have to buy a full sheet.

 

I have been doing a lot with Mach3 and CamBam and seem to be learning something.

 

Still having a bit of trouble changing the origin in Mach3 so that I can actually set X zero and Y zero where my stock actually is. For example if I have a drawing in cambam that does not have the edges lined up along the X/Y origins then I have a hard time placing stock on the table in the correct position. Still working on it though and youtube videos have been great resource.

 

Clay

[metalnwood]

If you surface the mdf so that it is flat you shouldnt have a problem.

 

MDF is good because it is cheap, it machines easy so easy to surface and when you cut in to it, which you will if you do any through cuts then when it gets banged up you take another half millimeter off it.

 

There is a reason why MDF is used as the sacrificial table on most CNC routers you will come across.

[Warhog]

I am going to get rid of MDF soon! I was just being lazy and using what I had kicking around. As my supplies keep building up I will make everything a little more "proper". I have received my order of cutters and the rowmark I ordered finally showed up. So things are progressing. I will see I they also have a crop that would work for the new base so I dont have to buy a full sheet.

 

I have been doing a lot with Mach3 and CamBam and seem to be learning something.

 

Still having a bit of trouble changing the origin in Mach3 so that I can actually set X zero and Y zero where my stock actually is. For example if I have a drawing in cambam that does not have the edges lined up along the X/Y origins then I have a hard time placing stock on the table in the correct position. Still working on it though and youtube videos have been great resource.

 

Clay

 

Clay

 

CNC certainly has a learning curve to it and it will take some time to get setup properly and establish a routine for consistant results.

 

CamBam uses the outline of the letter unless you are using stick fonts. When you want large sized fonts, choose Arial and pocket it. Otherwise use RomanS which is an AutoCAD font and then you can choose engrave.

 

You should always place your drawing with 0,0 at the bottom left when in CamBam. After you fasten you work piece onto the table, move your cutter to the same place relative to yoru work piece and then pick the x and y DRO's in Mach3 and they will reset to zero. Last thing is to pick the "recalc tool path" located under the window that shows your workpiece tool path lines. If you need to make a tool change, once the new cutter is in place and the z axis has been zeroed, pick GoTo Zero and it will move your tool into the exact same starting point. Do another recalc tool path and you are set to start cutting again. BTW, before picking GoTo Zero, ALWAYS move you cutter up from your workpiece a 1/4" or thereabouts, to ensure it doesn't drag through your workpiece.

 

You really need to have a good understanding of both software packages to obtain consistent results. Not only that, but trouble shooting will be much easier as well.

 

If you have access to a machine shop you might want to have them provide you with a 1/4" thick 12" square piece of aluminum that has a ground surface on both sides. When you want to engrave or make pcb's you fasten it to you table and then tape your work piece to it. I use a ground aluminum plate over my table. Btw, are you using the tape I recommended and are you covering the entire surface with it?

[ClayM]

Making some good progress! Got rid of the mdf. Managed to scrounge up a 12" x 15" piece of UHMW. Spent most of sunday leveling it. Takes awhile with 1/16 cutter and .005" stepover.

 

Warhog,

 

Turns out my local staples stores carry that tape! Works great! Thanks for the tip. I screwed up one of my first cuts by selecting the tabs in cambam thinking i need them. now i know why you said cover the entire surface. eliminates the tabs! Brilliant.

 

Here's what i have so far

 

 

More to come soon.

 

ClayM

[Warhog]

Well done Clay. Looks like you are now on the road to making your first panel.

 

Question...does the tape hold on that piece of UHMW. I ask that because I understand UHMW has a waxy surface so that could be a problem for you. If you try to cut something that requires more force the workpiece may actually slide on that type of material. Be careful.

 

Also, you may want to have some larger diameter cutters. As much as 1/16" is needed for most cuts, it would be a huge time saver to have a 1/4" and a .375" endmill for pocketing large areas. You will also want a 1/16" or 1/8" ball nose cutter.

 

How is your zeroing routine ...have you got that down now. Reason I ask is there will be times where you need to flip your workpiece to cut the back. You will need to re-zero it on a new zero point which brings me to my next point.

 

Dowel pins...they are 2" long and they come in a set with diameters incrementing at .001". Best to buy Chinese as they can be expensive. They come in a set

 

http://www.starrett.com/metrology/metrology-products/precision-measuring-tools/fixed-gage-standards/Pin-Gages#currentPage=1&displayMode=grid&itemsPerPage=24&sortBy=wp/asc

 

You will need these to help you in ACCURATELY registering a workpiece that you have flipped.

[ArsonsAngel]

Well done, expect more progress:thumbup:

 

 

 

 

 

 

 

 

 

sony z5 compact handyhülle

Edited September 16, 2015 by ArsonsAngel

[ClayM]

Thanks Everyone!

 

Warhog

 

Sorry, it might not be UHMW! getting my plastics mixed up here. I think its HDPE???

But the tape works great.Covering entire surface. Requires just enough effort to remove that you know it is holding tight but not a total pain in the ass to remove. I tried the regular spongy thick stuff before i found the tape you recommended and it was horrible.

 

Dowel pins sound good. I had been trying to think of how to register the flipped piece. So are you saying use dzus holes in the panels or just use edges of the stock?

 

Managed to get everything zero'd correctly (recalc tool path button does wonders) and even a tool change that worked great first try. Thanks.

 

Now that I've wasted a bunch of plastic (and tape) to get the hang of this I think I'm going to attempt the caution light panel. After a couple years trying to get it to work it would be nice to give it the finishing touches it deserves. I will need to flip this as well so I sense some more trial and error.

 

 

Clay

[Warhog]

Hi Clay...actually the term is pin gauges cause I'm getting old and I forget stuff which really sucks.

 

Anyways, you start by ensuring somewhere on your workpiece there is a hole in around 1/8" diameter thereabouts. It's not important what the diameter is since you will have a pin gauge set. Select the correct pin for the hole. Try and keep that hole to bottom left just as you do for 0,0. I also clamp a straightedge on the table that is perfectly parallel with one axis. With the pin pushed into the workpiece, I gently move the spindle head with pin chucked up in it and slide it tight to straightedge. When you' re done that, set zero in the DRO's and regen the tool paths.

 

Now I should regress back to your drawing when it's in CamBam. In preparation for using the pin for registration you need to ensure that the drawing your working with shows this hole. In fact this same hole needs to be at 0,0 on the screen when you generate the g-code.

 

If you want to check for accuracy, you can do a drill operation. Pick a second hole on your drawing that, like the registration hole, has already been cut. Select it and choose the drill operation but only have the drill depth set to -.0001. That way when you have your pin gauge still in the chuck you can run that little bit of code to move the pin overtop this second hole to see how accurate your workpiece alignment is. Move the pin down into the hole and if your workpiece is properly registered the pin should slide right in.

 

I don't like to use edges for registration as it's difficult to keep everything in position as your trying to get perfect registration.i get perfect alignment to .0005" using the pin method. :)

 

 

...the Caution Lights panel eh?

Tell me how you will make that before you start cutting anything. That panel is not so easy and I would like to see what your process will be. It might save you some major aggrevation.

[Stevos758]

I have the big brother the x6-1500GT,

 

Homing switches are a a great idea, mechanical or hall effect. I went with hall effect. If you are using mach 3 get the blue screen set by big tex. You can set up a touch probe for stock offset and a tool setter that makes changing tools easy. http://www.cnczone.com/forums/open-source-cnc-machine-designs/101878-cnc-forum.html

 

For software I recommend fusion 360. You wont get anything better for the price. Its amazing.

 

as far as cutting goes. make a sacrificial board. Mill it flat on the machine. Check out g wizard for feeds and speeds. Drillman 1 on ebay is an excellent source for cutters.

 

Looking good so far! good luck to you!

 

also I found scotch permanent double sided tape to be the best. the yellow kind. http://www.amazon.com/Scotch-665-2PK-Double-Sided-Office-Inches/dp/B001A3Q1XQ/ref=pd_sim_229_7?ie=UTF8&refRID=1ME5H1E8RFN317BET1C8

Edited September 17, 2015 by Stevos758

[ClayM]

It sure would be nice if I had more time try all the ideas being discussed here.

 

At this point time seems to be the enemy.

 

One thing holding me back a bit is " Cambam is thinking". I'm not sure if its a hardware issue on my end or software. I wanted to do a test/trial/see how it looks cut all the text on the CLP indicators.If I try doing POCKET on all the text in the same operation Cambam just thinks a lot and produces nothing. If i just try to cut 4 or 5 indicators it runs OK. From my experience so far i would think entire CLP will be around 25,000 lines of G-code!!! Does cambam have any limitations for any one operation?

 

Anybody here have this problem?

 

I'm going to try doing entire panel with 12 operations (so 1 row of indicators at a time). I will report back with the outcome.

 

Thanks for all ideas and advice everyone!!

 

Clay

[Warhog]

Pocketing is the problem. The only time you pocket is when your letters are at least .25" high. Most lettering is .15". Do not even think of pocketing letters that size. The caution lights panel should only require one operation... engraving.

 

I think you might be trying to do too much. What I suggest is that you send me your CamBam file and I will have a look at it and let you know what I think. I can also send you some of my files to have a look at so you can see how I am doing it. The only time I have to wait for CamBam to finish processing is when I am doing gauge faces. That's only because the lettering on gauges are much higher than normal panel lettering so I use a pocket operation to cut the letters.

 

Clay, send one of your typical CamBam files to me at jfw@cogeco.ca. I'll see where the problem is and get back to you.

John

[ClayM]

My thoughts for CLP is to cut multiple layers of something ( i have some 1/4" lexan)for the indicator boxes. Maybe 1/2" deep so 2 layers sandwich it together and paint entire thing with a few coats of black spray paint. next mask everything except individual indicator pockets. spray with gloss white paint. attach PCB with LEDs to the bottom and engraved light plate to the top. everything will be clamped together with the 4 holes that are in the lightplate. I suspect issues with light bleed from any gaps but i think i can seal it pretty good.

 

Clay

[Warhog]

Check this out Clay.

 

http://forums.eagle.ru/showthread.php?t=138862&page=5

 

Scroll down to my pics and you can see one way to make the CLP.

[ClayM]

As warhog stated I'm using the wrong font. Currently trying to get RomanS font installed on my CamBam/Mach3 pc. Seems like AutoCAD no longer supports trial versions for Win Xp 32 bit. I use another pc for autocad so it does have the RomanS installed but that pc does not have a parallel port. So.... still messing around with the issue of stick fonts. Funny how the little details always cause the most problems.

 

Also noticed some of the ballscrew support bearings where spinning in their bores. found there was x and y backlash that was not there before. I believe that the nuts used to preload the ballscrew support bearings are slowly backing off. So I took it all a part. Used locktite retaining compound on all bearing outer races. put it all back together and tightened up nylock nuts to set bearing preload. All is good.

 

I suggest anyone who purchases one of these ( cheap 3040 type cnc ) machines to check bearing fits for the entire machine and bearing preload on ballscrews.

 

Clay

[Deadman]

OK I am having a brain fart what is the CLP? and Why don't you just use the FOUR real fonts? Is RomanS the only font that you guys can get to work?