So, the question is about how people solve the problem, when they find , that there was some other tool path to be passed, but.... they just forget it or think about it later. In few words. I milled this plate And as you see it is out of cnc. Now I would like to make a chamfer. Is there any possibility make it? How to center it on the table? How to determine the coordinates of new placement? Please, can anybody describe the procedure as 1,2,3 how can I make a chamfer to this plate. I am not interested how it can be done theoretically and on the big professional CNC milling machines, but how it can be done using just C-beam router and some not very sophisticated tools. Thank You David
This is called registration. Basically, you need to be able to map the machine coordinates to the real world. There are three basic ways to do this. (1) Come up with a way to place parts repeatedly in the same place. Maybe drill holes to put locating pins in the bed. Or have two straight edges that form a corner you can clamp the item against. Then precisely figure out where that place is in the machine's space. Take a scrap and clamp it. Now drill a hole in the scrap and precisely measure where the hole was. Then you can do some math and figure out where the 'origin' is. Use GRBL working locations to establish that as the 'origin' and then you can now consistently register. You also need homing switches that don't move in order for this to work right. (2) Do a one-off registration. Clamp your piece somewhere on your bed. Then jog the head so that it is visually lined up with a couple of different known points like corners or the center of holes. Write down those coordinates. Then line up the cuts in your CAM program so that they have the known points at those virtual coordinates. Run your program. (3) Use a Pi Camera or some other camera to locate the piece on the bed. Either by figuring out the outline of the piece or by looking for fiducial markers. Then map the image or markers to the machine's workspace coordinates in some way. This is often how pick and place machines work. And some newer laser cutters and the like use this as well. But it is the most complicated to set up. So (2) is the easiest if you just need to do this once. (1) is the easiest if you need to do it again and again with items that are similarly shaped. (3) has the most flexibility, but is the most complicated to do. -D
Thank You Jonathon. May be at this moment (2) is really more easy to implement. Just do not like "visually lined" . Do You think that I can visually lined the end of the beat to one of the corner of this part and making chamfer, where even 0.2 mm will mater a lot. And something else. Ok, let's say I can lined visually end of my bit with some reference point. But how it will be the issue with X Y axes orthogonality? David P.S. May be using the cross line laser can help in this situation?
Tools can be of some help, but (2) will likely yield the least precision no matter what. To really dial in precision, you need to be able to do multiple trials with different scraps and tweak your settings until it is perfect. Then you don't want to repeat the process any more than you have to. So (1) will be more precise if you take the time to dial it in. You can definitely use tools to make your job easier. Calipers can give you a good idea of the thickness of the item. Touch plates or other methods can let you know where the tool head is in relation to the table. Aligning the x and y axes is harder. If you have a way of keeping the piece aligned to the x/y axes, then you just have to find one known point on it in relation to where the toolhead is. I've not done anything that required 0.2mm precision myself. Crossed lasers would probably help, but of course you would have to align them properly first and make sure they don't shift. -D
Thank You one more times. Should be rather creative process to implement double sided milling, I meant this little device cross laser Regards David
Two-sided milling is definitely tricky. BTW, you probably don't want a single cross-laser. You want two line-focused lasers. One aligns on X-axis, the other on Y-axis. Then where they cross is the center of the end mill. If you have a single cross-laser, then there is no way to point it at where the bit will cut in a way that is independent of material thickness. -D
I would suggest modifying the original drawing to include the chamfer and deleting all but 3 of the 5mm holes, keeping ones as widely spaced as possible. Set the holes to be re-drilled deeper where they cut into the spoil board. Have the program cut the holes first and then set the plate in place using 5mm screws pegged down through the plate and into the board. You'll still want to add clamps or hold-down screws as the 3 5mm screws will really only set a reference. Then run the chamfer. If you wish to chamfer the opposite side, same idea just create 3 new reference holes. Note, making the holes in the spoil board slightly smaller to where the screws actually thread in may help with positional accuracy (but I still wouldn't trust them as a hold-down). Rick.
HI, you do have the cad of the part? So here is what i do regulary if i need to mill two sides... should do for your problem as well: place your part with say the lower left corner at 0/0 in the cad, draw a rectangle around it which also has the lower left corner at 0/0 but is generously bigger at all other corners. now mill the rectangle out of some srcap material - make sure you cut an inside part!!! also make sure to activate the "cut inside corners" button - creating a temporary square edge to clamp your part against. clean your cutting area make sure there is no debris left .... now simply press your part against the ledge at 0/0 and clamp down. mill whatever you desire... hope that was understandable flo
Thank You both for response. So, before to ask about how people do double side milling, I of course had some practice. Unfortunately, this experience was not perfect at all. How I did it. In my cad file I had a part itself, and rectangular around it. Also , I had 2 holes at the center line of rectangular area, 5mm in diameter. Now, I had this cad , and I had also another one, which was the mirrored image of one original one. So, I fix the plate and mill just the rectangle and those 2 holes, making at the same time holes also in spoil board. After that I cut the part. After that I just mirrored the part up side down and run another tool path scenario which was just for making chamfer. The center of machining was untouched , the same, so everything should have been ok. But, despite of this pins, I could not position the part exactly at it's place. This little error in positioning course not successful chamfering.( some edges was not chamfered at all) That was the experience. After that I had realized, that the idea could work, but I have to find how to make this pins to be possible to position the part more accurately . So, that is why I asked about how people make it. May be there are some more smart tricks. I consider even to use somehow edge finder and center finder tools, but saw in some tutorials, that they can not be used in cnc routers, because of very high speed of spindle. So, thank You, guys, one more time. For this time I make chamfer with sander Regards David P.S. Ohhh, sorry, forgot to mention. Of course, I used tabs, when cutting part, so my part and rectangular around was one whole thing. t is important
