[RPCElectronics]

Looks great, no risk of chips getting up there.
Hoss

Thanks! I still have some cable management to do, plus I am looking for a keyboard/trackpad combo that I can mount right under the LCD and get rid of the keyboard and mouse that I am currently using. Ione has a nice wireless keyboard with a built in thumb-track device:

Wireless Joystick Keyboard, 2.4GHz, iOne, SCORPIUS-P20

My garage is small, so I have tried to use the wall mounting to my advantage with all of my bench mounted equipment.

[RPCElectronics]

When aligning the tool to the work piece, do you align the center of the tool to the 0,0 point on the piece? When using my 1/16" endmill, I was able to align it to the 0,0 point by eye and so far the cuts have been pretty good.

When I tried to use a larger 3/16" tool, I found that my cut's were pretty far off. I aligned the edge of the tool with the 0,0 point, to make sure the tool stayed inside of the cutting area. Could I get away with putting a fine tip pointer of some kind into the spindle, align that to the 0,0 point and then swap to the tool? Wouldn't that ensure that the 0,0 point is dead center on the cutter?

I did some Google searching for the answer before I asked here, but I could only find general CNC machine setups, nothing specific to the cutter alignment.

[hoss2006]

One of the most common ways is to use an edge finder to get to the center of the spindle on your 0,0 origin.
LittleMachineShop.com - Edge and Center Finder
Look at Chris's tips for a video on how it's used.
You can use your tool to touch off the edge too just remember to then move half the tool diameter in to get to the center both in the x and y.
Hoss

[RPCElectronics]

One of the most common ways is to use an edge finder to get to the center of the spindle on your 0,0 origin.

I have a center finder, but I don't have an edge finder. I'll pick one up.

LittleMachineShop.com - Edge and Center Finder
Look at Chris's tips for a video on how it's used.

Thanks, I'll watch this.

You can use your tool to touch off the edge too just remember to then move half the tool diameter in to get to the center both in the x and y.
Hoss

OK, so that means my original assumption that I center the tool over the 0,0 point is what I am shooting for.

Thanks, again!

[RPCElectronics]

I'm having a blast with the mill!

Only took me a week to start cranking out milled cases for my own products. I have been working with various outside machine shops for the last 10 years and now I can start doing them myself. I took a couple of videos of milling one of our recent products:

[ame=http://www.youtube.com/watch?v=mhoIh1ZJil8]CNC Milling - YagTracker Breakout Box - Radio/GPS/Power Side - YouTube[/ame]

[ame=http://www.youtube.com/watch?v=EKt9Wnil1kM]CNC Milling - YagTracker Breakout Box - YagTracker/GPS Power Jumper Side - YouTube[/ame]

I also built up a swingable keyboard tray for my new Logitech wireless keyboard/trackpad. I picked up a second LCD arm mount off of eBay nwe for about $15. I picked out this particular one because the VESA mounting plate can swivel up and down a full 180 degrees. This allowed me to pop-rivet the tray to the mount and then swivel it to the point where it's horizontal enough to hold the keyboard, but at an angle I can use the keyboard.

The tray was just some medium thick sheet metal I had left over from another project. I didn't have a break to bend the lip at the bottom, but I do have a Black and Decker Workmate, so I marked off the bend, clamped the metal in the Workmate and bent it that way. I actually ended up with a nice gentle curve in the bend, instead of a hard 90. The next step is to find some kind of material I can put around the lip's edge (So I don't cut my wrists on it!). We have some half-round plastic material that we use at work to line a hole cut in a panel, to avoid chaffing cables going through it.

Here are a few pictures of the mount:

[RPCElectronics]

Up until now, I have been doing 99% ABS plastic machining. This weekend I started into doing thin (~1.5mm thick) aluminum panel milling for some of my products. I think I have found some backlash. With the ABS, there was no real fight to mill the material, but even this thin aluminum is proving to be a bit tougher and now the backlash is starting to show.

Is this something I should consider to combat with Mach3's backlash compensation or should I look at re-loading the ballnuts with oversized balls? I'm just wondering what will be the best way to attack this. I was hoping that with the ballscrews I could avoid this, but I guess no amount of money makes you immune

[photomankc]

You can reduce backlash with oversize balls but unless you run double nuts it's not really practical to eliminate completely with oversize balls. Leads to binding. You really want to eliminate as much as possible mechanically. I think it's the biggest limiting factor right now in my tolerance. I can only reliably get to +/- 0.002" and that is right about what my backlash is. Compensation sometimes gets me great results and other times not so much.

I could go up a bit on my ball size and I think I will likely do that. Should be able to get the number down from about 0.003 to something with a 1 in the number and that would improve things for me. Compensation does worse and worse as the backlash gets higher. Compensation in LinuxCNC for 0.006" was not enough to keep bores and bosses from having rather strong quadrant marks.

[RPCElectronics]

You can reduce backlash with oversize balls but unless you run double nuts it's not really practical to eliminate completely with oversize balls. Leads to binding. You really want to eliminate as much as possible mechanically.

Yeah, I figured oversized balls were not going to be the only single, simple solution to the problem. I guess I was hoping that it might take out enough that I can live with anything left over. I'm starting to think that won't be the case.

I think it's the biggest limiting factor right now in my tolerance. I can only reliably get to +/- 0.002" and that is right about what my backlash is. Compensation sometimes gets me great results and other times not so much.

I might try out compensation and see if that can get me a little closer. You're echoing what I have read in many places: Mach3 compensation is either the Bee's knees or a nightmare. Depends on who you talk to, I guess.

I could go up a bit on my ball size and I think I will likely do that. Should be able to get the number down from about 0.003 to something with a 1 in the number and that would improve things for me. Compensation does worse and worse as the backlash gets higher. Compensation in LinuxCNC for 0.006" was not enough to keep bores and bosses from having rather strong quadrant marks.

I don't know if this will help describe what I am seeing as potential backlash, but this quick drawing might help:



The bottom left shows it the best that I can draw. I am using a two-flute 1/16" micro endmill for milling these 1.5mm aluminum panels. Running about 2500 RPM at about 1.5mm^second feed rate. The toolpath has it go in a counterclockwise direction (climb?). It looks to me like it plunges, starts the first side and works it's way around. By the time it's making it to the last side to cut, everything is slid over to the left just a bit and that causes this misalignment.

I have tried really hard to listen for missed steps. I adjusted my gibs the other day since I had way too much slop in the ways and I could literally "shift" the X axis back and fourth by holding on to the ends of the table and try to "rotate" it. It wasn't much, but enough to feel it. I adjusted the gibs to take out 95% of that movement. I then ran the bed X and Y in both directions several times the full travel to see if I had any binding or obvious missed steps. I didn't notice any audibly, but there is a chance it's happening. I'm considering loosening the gibs just a hair to see if my accuracy gets better ie. eliminating any missed steps that I might not be hearing.

[photomankc]

Tough to look at that and say sure this is the issue but I could see the lost movement stack up in a way that causes the little notch. I would test for lost steps by setting up on a fixed block and touch off an indicator to that and then run a loop of numerous back and forth movements. Make sure your final position is set in one direction with the backlash taken up. Zero the DRO and the indicator and then run back and forth along the travel. Coming back to zero from the same direction it should land on the indicator zero every time or darn close to it. If it starts accumulating error over time there could be some missed steps in there.

Running the gibs too tight can lead to stick-slip where the screw moves but the table doesn't because the friction is too high. It then builds up tension and only moves later by some unpredictable amount. This can look like backlash as well. I fight with that a bit too and I have tapered gibs that are far easier to set. It can be a really fine line to walk.

It's tricky though because a marginal setup might loose steps under load where it doesn't when just jogging around.

My thoughts on backlash comp is that it is useful to clear that last one or two thou but that's about all you should expect of it. These machines are likely going to have other error sources greater than that anyway so unless that table is perfectly flat, perfectly parallel and perfectly perpendicular, you are going to have dimensional tolerances to live with depending on where it's working on the table and where the overhanging weight is centered and so forth. Get the backlash manageable within few thou and use comp to take up what you can't mechanically eliminate. Get the gibs tight enough to eliminate what slop you can but not so tight that you can't easily turn the screw by the coupler. Don't obsess on getting a small cheap machine to crank out absolute perfection.

[RPCElectronics]

Tough to look at that and say sure this is the issue but I could see the lost movement stack up in a way that causes the little notch.

I completely forgot to mention that I milled the same file in some similar thickness ABS. The results came out perfect. No notch or any sign of missed steps/backlash.

I would test for lost steps by setting up on a fixed block and touch off an indicator to that and then run a loop of numerous back and forth movements. Make sure your final position is set in one direction with the backlash taken up. Zero the DRO and the indicator and then run back and forth along the travel. Coming back to zero from the same direction it should land on the indicator zero every time or darn close to it. If it starts accumulating error over time there could be some missed steps in there.

OK, I'll run this test when I have some time and let you know what I find. Also, I know this is unrelated, but is there an easy way to tell Mach3 to jog to a specific point? For example, I can hit TAB to bring up the virtual jog and jog it close to where I need it, but I can't get it to stop right on a point, even if I drop the jog % down to 5 or less. Is there a way to key in a specific X and Y value and have it "auto jog" to this point? It might just be a case of me not knowing Mach3 well enough yet. I am still using the stock screen layout and I think I need to look at tayloring more to what I use it for.

Running the gibs too tight can lead to stick-slip where the screw moves but the table doesn't because the friction is too high. It then builds up tension and only moves later by some unpredictable amount. This can look like backlash as well. I fight with that a bit too and I have tapered gibs that are far easier to set. It can be a really fine line to walk.

I was wondering if this is what is happening or if the friction is so much that it just misses steps and get's off alignment. Any suggestion on what I could do with the gibs I have or should I look into making new ones? I think I saw where many were using brass to make replacements.

It's tricky though because a marginal setup might loose steps under load where it doesn't when just jogging around.

I THINK this might be whats going on in my case. My only real evidence of this is that I can mill one design in aluminum and things are slightly off. I can mill the same design in ABS and it appears to be right on. I guess based on that, it might not be a backlash issue...

[quote]My thoughts on backlash comp is that it is useful to clear that last one or two thou but that's about all you should expect of it. These machines are likely going to have other error sources greater than that anyway so unless that table is perfectly flat, perfectly parallel and perfectly perpendicular, you are going to have dimensional tolerances to live with depending on where it's working on the table and where the overhanging weight is centered and so forth. Get the backlash manageable within few thou and use comp to take up what you can't mechanically eliminate. Get the gibs tight enough to eliminate what slop you can but not so tight that you can't easily turn the screw by the coupler.

Don't obsess on getting a small cheap machine to crank out absolute perfection.

I understand and accept that it's not going to be jewel accurate. I was just hoping that with the ballscrews I could at least turnout a cut out decent enough for an RJ45 connector to stick through, without too much gap. (The RJ45 is just an example of the many styles of connectors that we use.)

[photomankc]

For precise movement use the MDI window and give it Gcode. So after you zero the axis you can give it G1 X-10.0 F150 and that will move 10.0mm in the negative X direction at 150mm per minute. I assume you are all setup to operate in MM. That way you move it just as a program would. There is also usually a way (I don't use Mach3) to move in incremental steps per keypress so it moves some set distance for each direction key press. I prefer to just use MDI.

[109jb]

That drawing looks like an undercut from tool spring back. This happens when the tool is pushed away from the cut everywhere except where it dwells for too long. My guess is that you are plunging and retracting right in that corner so the tool essentially is dwelling there on both the plunge and retract cycles. Generally you want to plunge in the middle of the cutout and then move toward the cut line then move around and then move back to the middle before retracting the tool. Also, after the initial cut, make a clean up pass and see if that helps.

[RPCElectronics]

That drawing looks like an undercut from tool spring back. This happens when the tool is pushed away from the cut everywhere except where it dwells for too long. My guess is that you are plunging and retracting right in that corner so the tool essentially is dwelling there on both the plunge and retract cycles. Generally you want to plunge in the middle of the cutout and then move toward the cut line then move around and then move back to the middle before retracting the tool. Also, after the initial cut, make a clean up pass and see if that helps.

That's correct. The tool is plunging and retracting at the same point. I am only seeing this when I machine metal, not the ABS. Also, when I machine metal, the holes are always too small and don't come out correct width/height as in the drawing. I can confirm this with a few quick checks with a caliper or just simply trying to fit the part in the hole. When I test mill in ABS, everything is on par with the drawing and everything fits.

Having said that, I am using Vectric's Cut2D for my CAM, so I'll have to see what I have to change in there to produce a center plunge.

[photomankc]

Cut2D is extremely limited. I wish I had never purchased it. It decides where it plunges and has no facility for finishing passes at all. You can't expect to cruise through metal with small cutters in a single pass and have the dimensions match. I use CamBam and would normally run a profile with 0.007" roughing clearance and then a finish pass that takes it out to the proper dimension. Even on the larger mills if you just slot right through in one pass the finish will be rough and the dimensions will not be accurate.

Cut2D is fine for wood and soft stuff but I shelved it for anything dealing with metal.

You can fool Cut2D by making a Roughing tool that is say 0.010" larger than reality which will force it to leave some extra material then create a correct sized tool that you run a profile with at full depth and that will then fool it into doing a roughing/finishing operation. CamBam has that built in. You can easily specify the roughing clearance to leave on each operation from non to whatever you like.

[RPCElectronics]

Cut2D is extremely limited. I wish I had never purchased it.

In all honestly, it's really doing 99% of what I have wanted to do so far. With just getting started in this, the easy and rapid capability to produce solid toolpaths was really the attractive aspect of the software. Also, where I work, I ran into a guy at our airplane hangar, got on the subject of CNC and he gave me a 30 minute rundown of how Cut2D had changed his life in his side business of CNC banner cutting. It was completely random that I crossed paths with this guy. I don't know about the life-changing aspect, but he just about convinced me in that 30 minutes that Cut2D was exactly what I had been looking for. After a few hours of playing with the demo, I was sold. I didn't buy until recently, since I didn't have a running machine until recently

Cut2D is fine for wood and soft stuff but I shelved it for anything dealing with metal.

Agree 100% When milling ABS whether for an actual product or just screwing around with it, the results have been wonderful!

You can fool Cut2D by making a Roughing tool that is say 0.010" larger than reality which will force it to leave some extra material then create a correct sized tool that you run a profile with at full depth and that will then fool it into doing a roughing/finishing operation. CamBam has that built in. You can easily specify the roughing clearance to leave on each operation from non to whatever you like.

This is a brilliant work around! I'm going to try this tomorrow night when I'm not sitting at my bench with a soldering iron in my hand. Tonight is assembly night. These PCB's don't build themselves

[photomankc]

Hey if it does what you need and you can live with the work-around for occasional metal then that's great, save the money. I do lots of AL work and almost nothing in plastic so totally 180 from your boat. The main gripes I had with Cut2D were that it approaches metal cutting in ways that are not good for tool life, IIRC it has no canned cycle support for drilling, no control of how it enters and exits the cut, and I couldn't make any use of TTS tooling because it will not deal with a tool change so I needed 10 files to make all the roughing cuts and finish cuts.

It's not surprising. Vetric was aiming at the CNC router running in materials that they usually work in so that shows in how it approaches the work. If you ask them they will tell you that. When you cut metal you really have to factor in the fact that it never cuts exactly to size, the tool and the whole machine springs into or away from the work so you have to have a roughing/finishing pass on the pipsqueaks we use.