Jig&fixtures?UsefullTips?GCodeSubroutines?....

[TrickyCNC]

Is there (or should there be) a thread somewhere, that shows how to get the most out of your CNC machine ?

Most wodworking machines gain uses by adding jigs and fixtures

Tips for clamping , lining up, loading sheets,over the edge work, ...

Subroutine gcode for surfacing the spoil board, step and repeating parts, ...

anything else you can think of ??

[Dude22]

I have not seen any thread like that but I do think there should be, it would be very helpful to anyone who already has a cnc machine but wants to do some improvements. Aside from the ideas you had all I can think to add it dust collection systems.

[vtx1029]

great idea! I've always wondered why there isn't a show off what you've made area either...

[louieatienza]

great idea! I've always wondered why there isn't a show off what you've made area either...

There is a gallery in the Vectric forum, and many here (including myself) post some of our work in the build threads. But a dedicated thread would be cool.

Rich, there are some cool clamping tips but it requres some scrolling and searching. One popular one is to buy t-track that accepts standard 1/4" nuts and bolts. There are many aftermarket clamps and accesories made for them (check out woodpeckers.com for some ideas.) I'e also seen slotted tables which allow the use of standard clamps (make sure your tools are nowhere near the clamps or you'll see carbide flying around.) Same thing with 18ga pins; I use them quite a bit, but care is needed to avoid them at all costs! I've also seen t-slot wall material used, though it looks pretty weak. The garage organizer panels are made of PVC and look a little mroe durable. I use a grid pattern of 1/4" holes, and use 5/16" lag bolts to hold fixtures down. I even opend up a few holes and put threaded inserts for fixtures that I use very often.

Spoilboard level is rather simple, and it depends on the size of your table. But it would be pretty easy to draw a rectangle the size of your cut area, and do a raster pocket toolpath on it with your largest bit and big stepover. You'd find that you can leave a little ledge along each side, which you can use to reference your work parallel to an axis.

You could use work offsets to repeat a job in a different location, or simply zero out at a different location for a quick one.

[TrickyCNC]

Thanks Louie

I'm figuring things out as I come across them. Nothing major yet. I just thought it would be a good idea for a thread with it all in, so when you come to use your machine for the 1st time, you'd already know some tips and tricks to make things easier.

Rich

[ger21]

Tips for clamping , lining up, loading sheets,over the edge work, ...

Here's my tip.
I have fences along X and Y zero, for locating my parts. Both are set to zero in machine coordinates. My table has a grid of 1/4-20 threaded inserts, which I use to mount CAM clamps for holding parts against the fence.
I have my table (with fences and all the insert locations) drawn in my CAD program. I do one of two things.
1) Draw my parts and my stock against the X and Y fences.
2) I draw the part anywhere on the table I want, and bolt it down t the inserts. I use method one to drill the mounting holes so they line up with the inserts.

With both methods, the g-code is created exactly where the parts are drawn, which is exactly where I want them on my machine.

The main benefit is that I never have to zero the X and Y axis. I turn on the machine, home it, zero the Z, and start cutting.

The only real downside is that you can't really trim around the perimeter of a part unless it's bolted down. But, the only way to really do that anyway is to use vacuum.
And whenever I cut out something, I need to leave some material all the way around slightly more than the tool diameter, to prevent cutting into the fences.

Subroutine gcode for surfacing the spoil board, step and repeating parts, ...

You spend 5-10 minutes creating the program, and save it. There's really no need to go through the trouble of writing programs with subroutines, since once you write the program, it'll be run exactly the same. As Louie said, with CAD and CAM, you can create the program in a few minutes.

anything else you can think of ??

1) Learn your chosen CAD and CAM apps inside and out. Not just what all the buttons do, but really learn it. Learn how to write macros or scripts, if the apps support them. This can open doors that most people wouldn't even think of.

2) Read. Then read some more. Then keep reading. The Vectric and ShopBot forums have a wealth of information. I'd recommend going through them with a fine tooth comb, poking you're nose in every thread. If you're really interested in learning, then you'll learn a lot.

3) Watch how other people work, especially people that are good. You can learn things from others that you might never come up with on your own.

[TrickyCNC]

Thanks Gerry

I guess I was being too tight (trying to be efficient ). Trying to use the edge of the sheet as the edge of my part - no waste. I thought about adding fences, but couldn't figure how I wouldn't cut in to them when cutting off the edge of the sheet !

I know about using macros / scripts to make the cad do things it didn't know it could !, but as you say, you need to know the commands inside out.

I'll get reading reading reading ....


Anyone use their machine off the edge of the bed ? either with a lathe attachment , or another axis, or even just to cut dovetails or box joints ?

I have about 5" of X trtavel available off the edge, in anticipation for such things.

Rich

[louieatienza]

Some more stuff?

- Here's something I learned from a fellow Zone'r: When you have your feeds and speeds dialed in for a particular material and bit, write them down! This way you have something to reference to when the time comes again. Of course, even if you don't use EMC for spindle control, you can still enter a spindle speed in your CAM so that you'll have another place where that information is located.

- It's helpful to research your tool manufacturer's product, and see their recommended chiploads and SFM for their particular tools. These are normally based on 1X tool diameter for depth of cut. It may be difficult for most DIY machines to duplicate the DOC or SFM (surface feet per minute) that the toolmaker recommends, but you certainly can control the chipload, which should optimize both the cut quality and tool life.

- I've found that when adjusting for different tool sizes, depths of cut, feedrates, chiploads, I could do so roughly proportional amounts and get a pretty good result. So if I get a good quality cut with a 2-flute bit at about 8krpm, I could do the same with a 1-flute bit at 16krpm, or a 3-flute bit at 6.7krpm. Or I can run a 3-flute bit roughly 50% faster than a 2-flute bit, machine permitting. Or if my stepover at 1/8"doc is .035" (like I do for aluminum) I can go 1/4" at .017" stepover. This will take experimenting and maybe some broken bits along the way.

The feedrate formula is Feedrate = chipload * number of flutes * spindle speed. You can derive any one of them if you know the other three.

- Speaking of broken bits, I didn't know some places recycle carbide, so I stopped throwing them away.

- Related to chipload, if you research the math you'll see why you should decrease your DOC for profiling a percentage of your pocketing depth. This is because you're cutting with the full bit width.

- I've used single-flute spiral-O bits a lot for aluminum and plastic work. They work well with the higher speeds a router typically runs at (see above about chiploads.) Lately I've been using them on wood as well, as they cut surprisingly well, and it's easier to form a nice chip, and they seem to clear much faster. I even use a 1/16" single spiral-O for thin slots and detail work.

- When cutting soft aluminium (like 3003) I find it better to use a slow helix or even a straight flute bit, as it helps break up the chips.

- Use the shortest bit possible, and take the largest DOC your machine can handle, to decrease tool deflection.

- Scour eBay for deals on bits. I just bought 10 Kyocera 1/8" single spiral-O-flute bits for $29. They probably retail for that much EACH. I've avoided no-name bits for a long time; too many troubles. Onsrud heavily discounts bits, check them out (ebay handle onsrudcutter2010). I bought a couple 3/8" PCD bits for $49 each (polycrysalline diamond). They have a serrated edge, and I use them for cutting phenolics (specifically fiberglass-reinforced.) They retail at $620 EACH! But there's nothing better for cutting G10 Garolite. They wised up and raised the price to $99, which I think is still a good deal.

- If you use carbide-tipped bits, or insert bits, ger yourself a fine diamond grit whetstone; you can hone the flats of the bit when they get dull and get more life out of them.

- If your working with hard-to-machine materials, it's sometimes helpful to take an extra step and drill all the inside corners first before pocketing or profiling. This will help your bit, on the cleanup pass, from burying into a corner and potentially ruining your work, or bit breakage. Your router would thank you if it could.

- Here's a VCarve Pro trick, that would probably work for other CAM programs. Say you havev a sign with a large field and raised lettering. You want ot clear the field with a large bit, like 1/2", but you need 1/16" for the detail work. This would normally take a huge amount of time since the 1/2" bit cannot get anywhere near inside the lettering. The solution is to start off with say 1/4" bit, using 1/2" bit as the clearance tool. Then make another toolpath, with 1/16", using 1/4" as the clearance tool. You then delete the second 1/4" toolpath. You now have 1/2" roughing path, a 1/4" re-rough path, and you final 1/16" path. The extra toolchange is worth the huge amount of time saved.

[RossMosh]

Don't be afraid to use the router bit to index your jig.

Let's say you're cutting a complicated shape jig. Take a standard sized end mill and drill one hole a standard distance from the origin into the meat of the jig. Now you can put the jig anywhere on the table, drop the router bit down into your hole, and you're indexed and ready to go. You can do two holes on the same axis to confirm your jig is square to the router as well.

Makes engraving a finished board a snap.

[Vestus]

Hey Gerry, did you make or buy your cam clamps?

I'm new to CNC, but I did figure out one time-saving tip for 8020. As the slots are 5/16 wide, if you want to run limit switch wiring/etc down the slot, jam a piece of 3/8" vinyl tubing in to hold it in place. It's also easy to dig back out with a phillips screwdriver.

As this seems like a reasonable spot for future tips, I'll upload my dust shoe dxf once I finish tweaking it. It may take a few years though.

Btw, OrangeAluminum is the cheapest spot I've found for t-track: http://www.orangealuminum.com/t-track-1.html

[ger21]

Hey Gerry, did you make or buy your cam clamps?

I made them. Just a piece of pine with a bolt and washer.

[louieatienza]

Some more tips... some are probably painfully obvious, but those are the ones that tend to nip us in the butt...

- If you use certain bits, especially if you do this for profit, keep at least one and preferably a few backups. You never know when a tool may break, and it could be something careless like forgetting to zero out our bit, slug jamming a cutout, even a faulty bit. running out 5 minutes before teh store closes to get a new bit, or worse, waiting 2-3 days for a new one to come in the mail, frankly sucks.

- I keep all toolpaths for a job in a separate folder, and try to keep all operations separate, even if they use the same tool. This makes it far easier to re-run a particular op for whatever reason (see above!) I also number each op in the order I want to run them, and even put the tool in the file name, like "1 - Rough Pocketing ,250 EndMill" Note the comma. If I used a period, then everything past it would become the file extension. Then when you look for the file in Mach3, you won't see it and you'll wonder where the hell it is, until you change teh file extension type to "all types." Having the tool in the file name is a lot faster than looking at the program header in the g-code. In fact you can see all the tools you need without opening a single file.

- I had a block of wood that I drilled a bunch of holes, to hold all my bits and endmills. Makes it easier to see what I have (and what I may need.) Don't pile them in a box or a drawer; the edges of carbide can easily nick.

- I use a 60 degree drill mill to locate certain parts on my workpiece, i.e. center, with crosshairs I marked beforehand.

I like RossMosh's idea of milling a hole center of jig. One coulld go further by milling a larger hole, and then later on a probe can be used to find center.

- When you think you know it all, a situation will arise that will put you back in your place! You'll never stop learning something new. And even if you're set in your ways, always try different software, bits, materials... you never know what doors may open up.

- I force myself to not use my machine top as an auxiliary storage space or tool crib. It's so damn inconvenient to have to move all of that stuff to do one quick job.

- Make sure you clean your computer, keyboard, mouse, and drive of any dust or swarf (this comes from experience!)

- You can learn a lot from YouTube. Even watching commercial machines can yield insight into good machine practice. There are tons of resourceful people out there, and the tuition is free.

- DO NOT run your spindle, computer, dust collection, lights etc. off the same outlet (Don't ask how I know this one too...)