Thank you, Alex, I am not thing my steps/mm may not be correct. But I highly appreciate all the background.
Typing in commands will cause regular crashes, much better to use jog buttons and jog slowly (if continuous) or jog in known increments If you are in doubt about how far jog commands move your machine, perhaps it needs to be calibrated?
Thank you David, That is what I concluded just one chat ago, I think I must re-do the calibration. Thanks again.
While using the buttons, keep an eye on the Serial Terminal log to see what commands are sent - for your learning odyssey - nice to see how it SHOULD be done
Thank you great tip. And you again to everyone on this forum being so helpful to a newbie. I tried to use another system only two years ago and if you didn't have a Masters in Electronics the comapny was not interested in helping. The Openbuilds software and hardware is great and it is really good for this industry.
agreed, learn the basics sure, but offload the hard work to your CAM software. These days I’ve written a few gcode macros to perform simple 30 second tasks that I need to reuse, otherwise, I use CAM software.
When simulating the g-code, the simulation window shows a 100 mm x 100 mm area. Is it possible to reduce this or is it picking up these dimensions from an internal setting? Can it be changed? Thank you.
those come from the machine setup, what are your GRBL settings for max travel? settings $130 to $132 mine look like this on this test controller $130=810.000 ;X-axis maximum travel, millimeters $131=730.000 ;Y-axis maximum travel, millimeters $132=90.000 ;Z-axis maximum travel, millimeters
That is strange. Based on the attached g-code file, I do not see how the X and Y-axis could have such large dimensions. I am missing something.
I suspect that the envelope of that gcode program is so small that Control just gives up trying to scale it and defaults to something it thinks is sensible. You can zoom in and tilt the preview if you have a 3 button mouse with a scroll wheel. You really should specify G90 or G91 in your program (and I would also recommend getting rid of that G92 - It will come back and bite you sooner or later. You should achieve the same thing by zeroing out the axes in Control at the point that you want the program to start. ) Beware that GRBL has some built-in tolerances for calculations that are of the order of a few microns. If you want to carry out movements of that order with accuracy, you may have to fool grbl that your machine is bigger than it is (e.g. reduce steps/mm figure by a factor of 1000 and program millimetres for microns), but that's getting really off-piste for someone new to this.
Thank you, Misterg, Thank you for your points of view. To your point about the micron movements I want to make, should I do what you are suggesting i.e reducing the steps/mm by a factor of 1000 and then write the g-code in mm? What about the GRBL settings such as: $11=0.020 ; Junction deviation, millimeters $12=0.002 ; Arc tolerance, millimeters Should I adjust all of this? My application is very specific, I understand that.
I would say not. The effects aren't well explored and it may well cause other problems with the precision of the internal calculations. In fact, I would get the whole machine working with a test program for something at least ~10mm x ~10mm, using completely standard settings before changing anything.
Hi Misterg, I believe your idea of reducing the mm/step by a factor of 1000 and then multiplying the g-code by 1000, is a good idea for this machine with such small travel and the intent of running micron steps. Probably should have steppers with 0.9 degrees per step, instead of the standard 1.8 degrees per step. What are your thoughts or opinions?
No, this is a really bad idea as the torque on 0.9 degree steppers is much lower than on 1.8 degree steppers. The resolution of 1.8 degree steppers with 1/8 micro-stepping is more than enough for even the smallest detail a hobby CNC machine could produce.
I need to know more about the entire system to understand how exactly you are achieving such small movements. motors (200step per rev), microstepping (stock 8x in the BB?), any gearing, leadscrew pitch? and, where did you get an endmill that can mill an 0.01mm hole?
Hi David, My apologies if I confused you. It is a 1 mm diameter hole, I am milling out with a 0.6 mm diameter end mill. I have 6 mm dia. 1 mm pitch pre-loaded lead screws on each axis, which are directly coupled to the Openbuilds Nema17 stepper motors, controlled via the Openbuilds X32 Blackbox controller. I have attached a photo of my machine. My machine's purpose is to be used for the following operation as this is for my part-time postgraduate studies. The machine's sole purpose is to conduct tests as shown in this video. Now instead of 6 fluted dove tail like cutters you see in the video, I will use 2-fluted end mills. I hope all this info helps and thanks again for all the advice.
Thankyou In light of this and having reread the Gcode you posted, which only moves between -0.005 and 0.005 in X and Y, which woudl be a 0.7mm hole with that 0.6mm cutter..... I think I see some things you need to think about and experiment with. 1 - stopping the drill while still in contact with the workpiece. I believe this will skew your strain readings. There should be a Z lift between each cut level from this Code: G2 F17.00 X 0 Y -0.005 Z -0.0100 I0 J0.005 G1 F17.00 X 0 Y 0 Z -0.0100 M3 S0 (Spindle will turn-off!!) G4 P 30 M3 S40000 (MSG, Take measurement!!) G4 P 10 G1 F2.50 X 0 Y 0 Z -0.012 G1 F17.00 X 0 Y -0.005 Z -0.012 G2 F17.00 X 0 Y -0.005 Z -0.012 I0 J0.005 to this Code: G2 F17.00 X 0 Y -0.005 Z -0.0100 I0 J0.005 G1 F17.00 X 0 Y 0 Z -0.0100 G1 Z0.2 ; lift out of contact so cutter is not placing pressure on workpiece during measurements M3 S0 (Spindle will turn-off!!) G4 P 30 M3 S40000 (MSG, Take measurement!!) G4 P 10 G1 Z-0.01 F2.5 ; feed back down to previous level G1 F2.50 X0 Y0 Z -0.012 G1 F17.00 X0 Y-0.005 Z -0.012 G2 F17.00 X 0 Y -0.005 Z -0.012 I0 J0.005 2 - the straight down plunge will be placing huge strain on your machine and not cutting as deep as you think it is. endmills , despite the name, do not drill very well so you want to avoid a direct plunge. Much better is a ramp movement Code: G2 F17.00 X0 Y-0.005 Z -0.0100 I0 J0.005 G1 F17.00 X0 Y0 Z-0.0100 G1 Z0.2 ; lift M3 S0 (Spindle will turn-off!!) G4 P 30 M3 S40000 (MSG, Take measurement!!) G4 P 10 G1 Z-0.01 F2.5 ; return to previous cut level ;G1 F2.50 X 0 Y 0 Z -0.012 do not straight plunge ;G1 F17.00 X 0 Y -0.005 Z -0.012 do not cut directly along the radius G1 X0 Y-0.005 Z-0.012 ; ramp from Z-0.01 to Z-0.012 while moving Y from 0 to -0.005 G2 F17.00 X 0 Y -0.005 Z -0.012 I0 J0.005 3 - even better is an arc to enter the cut, and a helical ramp, I will send Gcode for this tonight that is generated by SketchUcam, the Gcode plugin for Sketchup, I just don't feel like hand coding it (-: Basically a half circle arc from the center point to the start of the cut. Then the cut itself is an extension of this arc and the machine does not have to stop to turn the corner, making the helical entry and the cut into one smooth motion. Note you do not need an F word on every line, it is modal so stays set after the first setting, so you only need to give it when the feedrate changes. Makes less work for the controller to process each line, and more usefully, makes the Gcode easier to read when there is less of it (-:
Hi David, I am so appreciative of your input and help. It is highly appreciated. You are 100% correct. I had forgotten that the cutter should be raised slightly, as it could pressure the workpiece. Thank you for spotting that. I would like to see the new g-code you generate. Could you share the associated Sketch-up and CAM files? In regards to the g-code that you were going to assist me with generating, I just wanted to let you know that the depth increments I would be using are as follows in mm: 0.00 0.01 0.02 0.03 0.06 0.09 0.12 0.18 0.24 0.3 I will then conduct test runs to test the g-code. Which version of Sketch-up must I use or buy to use the CAM? I have used software by the name of CNCcookbook GWizard to calculate the speeds and feeds for this 0.6 mm 2-flute end mill for Grade 5 titanium. It is predicted to use 16 330 rpm for the spindle speed, an X and Y-axis feed rate of 36 mm/min and 18 mm/min for the plunge feed rate (it changes to 36 mm/min for a helical entry). See the screenshot from the program attached. Do these seem reasonable? The idea, of course, is to not introduce additional residual stresses from the machining process before measuring the previously induced residual stresses. And one other question: Is it worthwhile reducing the step/mm by a factor of 1000 and then multiplying all g-code distances by 1000 to avoid any internal tolerance issues that I have been warned may occur? I did try this yesterday for the machine, and to me, the machine appears to behave better, and the stepper motor temperatures are low. But maybe it is just my perception. What are your thoughts about this? And once again, thank you for all your guidance and support.
I will SketchUp Make 2017, the free version is all you need. Sketchup Make 2017 (Last free version) SketchUcam is free Releases · swarfer/sketchucam yes, cnccookbook is probably correct BUT it assuming you are using a Haas or at least a Tormach mill so may be too fast for your machine (stiffness of the machine). You need to listen to your machine cutting, put your hand on it and feel for vibration, and try different speeds to get a feel for how your machine reacts. And, titanium! yikes! that will wear out the endmilll quite quickly so have many in stock and change them often. If you can see edge wear under a microscope it is blunt and will affect your cuts and your strains. This is a nice expose of titanium cutting , a perhaps some fo John's other videos on cutting titanium will be useful to you. This came up because the Gcode you posted had XY motions of 0.005mm but now you say you are actually cutting larger holes than that, a 1mm hole with 0.6mm cutter, so 0.2mm each side of center which is much more reasonable given your hardware. 0.2mm is 320 steps which should not be a probem for a Blackbox X32. So, no, not worth the effort and potential mistakes to be using a multiplier on everything.
Thank you again, David, I will also adjust for the smaller, less stiff machine. Thank you for the videos, I will check it out and start testing.
Thank you for sharing the video. I can see how the helix descending is a good approach. But as mentioned could increase the wear. An important important for me is that I will replace the end mill every time I do a new hole (measurement). I will look at his other videos. Thanks again.
Here is a diameter first mode hole drill operation. 0.6mm bit, 2mm diameter hole, 33% step over Note that this cycle (diameter first) first does a helical bore to full depth at 2x bit diameter (you don't want this) before doing each layer out to diameter (you want this) in a spiral. The spiral is really 2 half circles, start point (Y) to Y+stepover/2 then to Y-stepover for each rotation. The other option in SketchUcam is depth first, where it will do a helical bore to full depth for each step outward. Neither is exactly what you want, but the idea here is education not a complete solution (-: Exactly how it generates the hole boring depends on the bit diameter, hole diameter and stepover% if hole diam < 2x bit diam then it always does depth first (that is why I had to do a 2mm hole here, 1mm always comes out as helical bores to depth. if stepover is less than 50% then it always helical bores first, never plunges, deeming this a 'for hard materials' operation if stepover is > 50% then it will plunge the center of the hole to depth, deeming this a 'soft material' operation. SketchUcam was born in the world of cutting foam board to make RC airplanes so this makes sense in that world, you can cut foamboard at pretty much any rate you like, plunge with almost any tool etc, very forgiving. Titanium, not so much (-: Note that there are limits as to what you can do in Sketchup at the small end of the scale because it does internal comparisons to 0.001 inch, if the difference between numbers is less than that then they are regarded as equal. SketchUcam code does comparisons to much less than that (I had to write my own function for it), but now and then the Sketchup comparison will mess you around.
Hi David, I see your generated G-code has a G3 G-code for a counter-clockwise arc, is that not "climb milling"? Is that suitable for this application? I am asking as I have seen several recommendations for conventional milling to be used. Thank you again for the assistance and insights. I have got Sketchup and your CAM extension work. Really great system, thank you. Did you use the pocket option to create the tool path?
I did not deliberately select a direction (-: Climb milling it generally good for metals, conventional is good for plastics and foams, but it does depend on the machine too. On my machine I use them, in part, to achieve the fit I want. My machine is belt driven and has a little flex in it, so climb milling will leave the part large and conventional will leave it small. I did some parts in plywood recently where I climb milled to depth and then did a finishing pass at full depth and conventional direction, leaves a very smooth surface. No, it is a 'plunge bore' operation, specifically for making round holes. There is a playlist (-: https://www.youtube.com/playlist?list=PLm728rLHCWOw-vRvTJwS_5MmKG1fs4sZ0
I am helping someone with a Shapeoko XXL machine. He likes how the OpenBuilds controls my machine (CNC4NEWBIES 51x53) Has anyone used the Openbuilds software package on a Shapeoko xxl machine and how does it compare with the Carveco motion that comes with the machine. Will he still be able to use his tool setter and can make his 0,0 in the front left corner of the machine? Most of his designs are done on Vcarve Pro. Thank you! Mike
