I've got Lead 1010 and I use cut2d pro. Everything works great, the etges of the material are smooth except the tabs. The last pass is set to 0.13mm- it smoothes the edges but I think this pass makes the grooves by the tabs 3d (I'm attaching a photo). What can I do to make the space by the tabs as smooth as the rest of the edges?
You have 3D tabs selected in your setup - you don't need that for a 2D model. Also the tab is overly thick. I would de-select "3D" and set tab thickness lower, say 1.5mm or so. I don't use Cut3D and I'm guessing language translation from the graphic picture.
Which direction is that last pass? What you are seeing is the result of backlash and toolpressure relaxing when it slows down to cut the tab. A climb cut as a final pass might alleviate it, ie set 'stock to leave' for the initial cut then do a final pass at full depth to remove that stocktoleave.
so I've tried several things: • setting an additional finishing path after cutting the element to run 0.13mm less than normal- it didn't help. • I've made the last finishing pass run reverse, and I lowered the height of the tab to the height of the last pass and it's much better but instead of the grooves I have bumps now
The machine is flexing from tool pressure, I know because my machine does it, those exact sort of dents at tabs. I have not seen that sort of smooth lump though, I think that means you have a lot more flexibility than you should have. The tool is rotating, so if you picture it cutting a slot going away from you, the front of the tool is moving left to right, forcing the tool to the left (in the photo it appears the bit is moving to Y-). What can you tighten to prevent that?
It may be the machine, you're right.. I've tighten the Z axis as well as X axis (hope I did it right ) Should I tighten anything more? I also have a question regarding the cutting setting to you- an expert, could you share what setting do you use for cutting MDF board?
18000rpm, 0.1mm per tooth. calculate feedrate from that and tooth count. it must chuck chips not dust. so for a single flute 2mm cutter that is 1750mm/min feedrate, 1.3mm deep per pass. Could go deeper or faster but delivery on the 2mm cutter takes weeks so I am somewhat gentle on it. Bigger carbide cutters can go even faster if the machine can do it. With our relatively lightly built machines we must embrace the principles of HSM, "fast and light", so small depths of cut at high RPM for a light cut at high feedrate.
I've tried your settings ad it's much better- thanks! How do you calculate all those settings? I've got a striaght 2flute bit 3,175mm?
I use the calculator built into SketchUcam. But there are plenty of them online, but it does boil down to finding a starting point, then fine tuning for YOUR machine and making a note of the things that work. feedrate calculator cnc router - Buscar con Google
