Hi All - Just wanted to introduce myself as I've just completed my build. Here are the details: Sphinx 1000x500 build w/ Limit Switches 800w Water Cooled Spindle CNC xPro Board - Hint, $4=1 - That had me messed up for about an hour Nema23's Fusion 360, and GRBL Panel I had a long weekend of struggles in learning how to get coordinates setup, stepper motor steps adjusted, machine homing correctly, etc. All in all I would consider it a pretty good success. Got some test routing done and didn't break any bits yet. One of the projects that I plan to do is routing recessed holes into some aluminum plate. The aluminum plate will already be final sized. With that said, I am trying to find out how to do my G54 offset properly, as I want to ensure the holes will be exactly where I expect them to be. So, in determining 0,0, where would the bit sit. The model has it in the lower left corner. My question is a bit more precise, meaning, would I sit the bit inside the corner, outside on the corner, half on/half off the corner, etc. - Edit: In further reading, it would appear the the 0,0 point is the exact center of your bit, in both directions. Thus, it would seem the center of the bit would be placed right on the corner? Right?
Once you have made your machine as precise as it is going to be, consider using the machine itself to help you set up the proper stops. So, for example, set a stop of a relatively soft material approximately where you need it. Then create a profile which will cut through that material at a precisely known coordinate location. Then you place any stock against that stop when clamping it in place. And you know that the edge of the stock is precisely located at that known coordinate. Then you drill holes or cut shapes accordingly in your software. If you have homing switches, those stops can be permanently installed on your machine and can be used for precise placement of any other jig or template you put on your machine bed.
Thanks Joe for the reply. That is so far what I have determined based on quite a bit of reading. Appreciate the help.
Cutter compensation is part of calibrating your machine. When you set up your software to cut, you need to tell it how big the bit is. Then when it is cutting the outside of a shape, it can offset the path by half the cutting diameter to give a precise outline that you want. But you don't want to just use the manufacturer's specs. There are various factors that can modify the effective cutter compensation to be larger or smaller than the factory specifications. For example, I do most of my cutting with a bit that is 2mm wide. Some factors (like the runout of the spindle) make it cut in a diameter that is slightly larger than 2mm. Other factors (like the dullness of the bit or the nature of the material cut) make it cut in a diameter slightly smaller than 2mm. The only way to know is to cut a slot in material and then measure the width of that cut. The width you measure is what you specify as cutter compensation in your software. In my case, even though I have a 2mm bit, the actual cut width is closer to 1.9mm because the material I use is slightly springy and so deforms just a bit when it is being cut. For other materials (like metals), the runout of your spindle will probably dominate. But the only way to be sure is to measure. -D
Thank you for the information, that is a good explanation. Would that, or wouldn't that be achieved in the software? Meaning, when I tell Fusion 360 my bit information, is that already written into the gcode? I understand the part about the actual size the cutter makes versus the advertised size.
Accounting for cutter size is entirely done in the software. So when you generate your gcode, the paths there already account for the assumed cutter size. And if you change cutter size, you need to re-generate your gcode.
Ok, in looking at Fusion360, I've been using the "In Computer" Compensation type. I'm assuming this is what I want to do, and obviously the accuracy is contingent on the actual size that the bit cuts in the material versus the advertised size.
Wanted to provide an update - Was able to get the 8x10 2D contour pass perfect. However, there are 12 holes that are made using 2d adaptive clearing, that continually come out too small. I've checked my F360 options,and am NOT leaving any stock. I'm at a loss on this. The holes are slightly undersized.
Some controllers will allow you to adjust the tool offset for the diameter/rad of the tool and do the math to adjust the tool path. I looked around and didn't see it for any of the GRBL software controllers. I use mach3. If a pocket or slot comes out small(ideal case) then I make an edit right at the controller and rerun the code til the size of the feature is where I want it. No need for me to have to regenerate a new toolpath in CAM. I'm not up to date on GRBL, its use of the D term for G41/G42, or if there are any work arounds/scripts for this. Last I knew it doesn't support 41and 42 and the toolpath isn't adjustable on the fly. Offsets are generated in the output and are final. Maybe one of the GRBL gurus can chime in to check me on this. Basically you don't want to have to go back to your CAM software to edit then regenerate all new code to dial in a tool, but if you have to then you have to. BTW, all this is assuming the machine has been calibrated.
Thank you for the input, I'm trying to learn as much as I can. Here is some additional fun facts that might play into things. 1) My spindle rotates ccw. It has the ability to go in the other direction, but I thought it was worth mentioning. I have been using it in ccw rotation. (My manual mill rotates cw.) I'm starting to think that is wrong, and it should be going cw rotation. 2) Ran the part again, everything is perfect, however in order to get the holes right I had to add(remove) negative stock. What is strange to me, is that the outside cut out, the 8x10 is precisely that. As noted there are 12 holes, all are exactly spaced as per the CAD. Machine has been calibrated to my best ability. Both axis' were measured to their fullest, and movement is exact to the mm over the length of the access. I used a ruler, and a .1mm v-bit.
So you have been cutting with the bit in reverse.....? How are you measuring this? How much more did you have to cut? Aside from other things, the structure of the machine, the tool, runout, etc all have different dynamics in linear cuts verses circular cuts. I can get into more details as to why, but I'd rather refrain from tailoring an hours long written article on this. Just know that if you're seeing a hairs difference then this is likely the case. There could be a software and controls side to this as well in regards to how circles are handled as lines or arcs. You should borrow or purchase a dial indicator, a dial test indicator, or should already have a set of calipers laying around. A rule doesn't have the resolution to calibrate these machines for the tolerances you're looking for and every eye is subjective(even when looking at dials. Although dials bring it in a lot closer than a rule). DIY Machine calibration is a pretty highly covered topic at this point. I recommend you check out as many vids on this by people not using rules, but something more accurate and precise. It is also good to know what resolution your machine and settings are at before chasing that Dragon. Joe
1) Yes apparently so. I don't know how much that is contributing to any error rates that I'm getting. But again, the only error I can see is on the circles. Edit: Just went to rewire the spindle, the directions from the place I got it from were not correct. 2) The outside 8"x10" is measured by rule. Edit - I now have used calipers and confirm 8"x10" exactly. The circles I did negative stock of -0.35mm. 3) I have all of the mentioned tools, I am going to get a longer set of calipers.
I'm lmao. Okay CNCMD. Get that spindle wired correctly and let me know how it cuts in the other direction. Still lmao. No offence. I'm really here for ya. Update when possible.
No offense taken, I'm laughing at myself. I can tell you that now the 3.175mm bit cuts exactly 3.175mm. So that takes the variance in the bit size out of the equation. The holes are still slightly out, .20mm. I'm going to revisit my stepper steps using a caliber this time, I can only do a 6" span, but its worth while to verify. I'm going to get a 12" set soon. Thanks for being here for me. I think I've been working too many late nights...lol.
Further updates: Ok so, I finally caught onto the fact regarding the use of a dial indicator over a rule. I would say there is as much misinformation out there as there is information. I've honestly googled and found countless calibration exercises using a rule. Since I honestly own quite a few measuring tools, I broke out the digital dial indicator and used that to calibrate steps, and as expected by Joe, there were variances found. Ironically the first noted variance was about 0.35mm, which was the amount that I was adding as negative stock removal. Coincidence? Maybe. But probably not. All in all I was able to go though all 3 axis' and each one of them were off by some amount. So I can report in that I feel my steps are now correct. I need to re-run the part, and see what the overall effect is.
Just wanted to provide an update, I've had some good success lately with the machine. Got my first aluminum parts cut. Cutting aluminum is pretty challenging, I'm trying to work on feedrate settings, and depth of cut.
I know you have calibrated your machine now, but I thought I would throw my 2c in as to how I calibrated mine for others. I used a set of digital callipers, opened up to their fullest extent, duct-taped to the carriage and then an object (I used a block of 4x4) put up against the 'head'. Zero the callipers digital readout and instigate a move less than the extent of the callipers (in my case 10cm), then read off the calliper how far you moved - do it a few times in each direction, each time updating your controller's scale setting and you will be pretty close to spot on. Bush engineering, for the bush
That's a good technique. Looking back I was purely in a rush to get cutting. I ended up doing fine with the digital dial gauge that I had. I used a drop in T-Nut, and positioned it on the axis that I was trying to calibrate. My issue was really in the backlash. The Positive move, going say into the dial was spot on, however, when returning "back to zero" the move was different, and it didn't return to zero. I had to adjust the backlash nuts, and its been good so far. I am actually getting a new bed surface on Monday. I went with 1/2" ATP-5 plate. I am going to have this just sitting on the frame of the machine since it weights 35#'s its not going to move. I am then going to screw down 3/4" mdf to it. And then add T t tracks on top of that. The actual sacrificial surface will be 1/2" mdf that will sit in between the t-tracks. Pics to follow next week.
35lbs of steel on aluminium will move, easy. It’s not the weight, but the contact area friction that determines that and there’s not much in the v-track to steel.
