Hi. My lead 1010 used to make perfect holes. Now all im getting is oval or egged out holes. Something has obviously loosened up or moved and Im in the process of tracking it down. The holes are oval and it's always in the same direction which is 1 o'clock or along the the y axis slight turned to the right side of the machine. Just curious what you guys have to say?
Ok but does the direction of the egging indicated the problem is in or with the right side y axis assembly?
Check the bearings, lock collars and especially the motor coupler on the X axis - assuming that your pic is oriented with the Y axis vertical. Motor coupler slipping is the most likely cause for that amount of backlash. Also check that your machine is still square. Alex.
So I went over that machine and I can't find anything wrong with it. Good news is the holes look really good but they are always a bit undersized now. A 1/2" hole .500 will turn out .492 -.498" in that range/ Checked with a digital caliper. Also checked size using CNC bits the same size as hole. In WOOD. I do have 2 videos I made... I have a question about WHY the machine is doing what it's doing. Will someone there at Open builds take a look? When boring holes the machine will slow down doing very short moves to make a circle but then speed up or it will go full speed feed rate to depth. It's all over the place. It's never consistent. What gives?
please tell us your process, which CAD software, which CAM software, and attach a screenshot of the drawing and the Gcode you are using.
Fusion 360 for CAD and Cam. Using Bore which does a spiraling helical cut and stays in contact with the selected hole surface, For example I would use a 1/4 " Spiral bit to bore out a 1/2" hole. you want me to attach gcode. file or paste code into message?
If you have got rid of the backlash the next step is calibrating your machine (Calibrating your cnc) the pdf explains the theory, the wizard in Openbuilds Control (see the video in that link) makes it easy by doing the sums for you. Calibrate over the longest distance you can measure accurately, 100 mm is not long enough. Upload your Fusion file and we will be able to explain why it starts a bore toolpath slowly and then speeds up. Alex.
yes, please attach the gcode file meanwhile, you may want to enable smoothing, this reduces the number of short line segments making it easier for the controller to process the lines really fast. (not just Blackboxes, all controllers can be overwhelmed by many small lines)
In the file you posted above, you have the boring operation set to 'use ramp' at 2° down to depth; and the ramp feed rate set at half the cutting feed rate. So what the machine should do is to spiral down slowly to the full depth of the hole, then it will make a full circle cut at the normal cutting speed (so will speed up). If you have checked the 'finishing pass' box (which you haven't in the file above, but it sounds like you may have done at some time), the tool will retract, then plunge the full depth of the hole and make another full circular cut. It sounds like the machine is doing what you've asked it to
The problem with that is is that it doesn't slow down sometimes it will go full feed rate randomly. I have a video showing what it is doing. It will literally make on hole half feed rate and then on the next hole go full feed rate and it also randomly does both even on the same hole. There is zero consistency.
It's not your g-code - there is only one feed rate specified in the file you posted, and that is quite slow, so your machine is not doing what you have told it to. Was that definitely the file that the feedrate varied widely with? Alex.
in the gcode I see that some holes (top left) are being cut with arc commands and some (top center) are being cut with many small line segments, not arcs. do you see these speed differences between top left and top center?
I looked at the video and the center 3 were done following the settings. Half the feed rate with a full circle at the end. The last 3 were not. Bored out at full feed rate to depth. I did not change any settings.
I haven't seen the video, but there's something funky going on with the post processor: I post-processed your f3d file with both the Open Builds one and the default F360 one. I got the same results as your 'holes.gcode' when using the OB post processor, but something much more sensible from the default F360 grbl post. Here they are plotted using NC Viewer: This is from the OB post on your 'test v9.f3d' file (same as your 'holes.gcode' file) - the file is ~6500 lines: For the first 6 holes, most of the path is very dense XYZ coordinates, but towards the bottom of *some* holes it switches to arcs for a varying number of rotations. The last 3 holes use arcs only. This is from the F360 POST from the same 'test v9.f3d' file - it is 630 lines: You could try the F360 post processor to see if things are more consistent.
