Could someone please give me some advice with the workflow from Fusion and the manufacturing process on the machine? Machine: TTC 450 pro I wanted to machine a test piece, and now I am really stuck. See the pictures and the gcodeFile.
This looks like a 'feeds and speeds' issue to me, rather than workflow (workflow seems OK?). Is this the machine? Twotrees TTC450 PRO CNC Router Machine If so, it is quite lightly built and the spindle is very small / flexible, so you have to take gentle cuts, and take some time to experiment and find the cutting parameters that work best with it. Try drastically reducing your depth of cut / stepdown - it looks like you're taking a 1.6mm deep cut with a 3mm end mill - try taking 0.1mm deep cut and see if you get better results. If that works OK, try 0.2mm, etc. I would also stick to 'climb cutting' for the adaptive toolpath. From looking at the gcode, I think you have it set to 'both ways' at the moment. It's likely to give poor results with a light machine as the deflection will show in the result. As a side note: AFAIK, the 2D toolpaths in Fusion360 aren't 'stock aware' - I tend to use 3D adaptive (followed by 2D Contour), even for 2D type operations as it avoids unexpected collisions. I think there are more / better options for setting step-down, too (I haven't got it in front of me, and I know that Autodesk have been changing some things around recently.) Have another go, and if you get stuck with the Fusion side of things, post up your work file and I'll take a look.
Thank you! What I don't get: Why is the deviating that 'huge', I assume that gcode bases on absolute xyz-values and are not depending on the previous value. I renewed the post process files, once with OpenBuilds and once with Grbl. I compared them and they are not same also apart from the header – why? For the controller I have OpenBuilds CONTROLER, gSender and UGS at hand. What do you recomend?
My impression is that the machine was being overloaded and skipping steps (so it could end up anywhere!). GCode can work in both incremental and absolute values (G91 vs G90), but the programs you've posted all use absolute mode (see the 'G90' near the top of the file). The two post processors use differing strategies to turn a toolpath into gcode. For example: one generates the initial helical path using circular arcs (the 'I's and 'J's ), the other uses short line segments, etc. The resulting tool movement will be the same (to all intents and purposes), but the gcode looks very different. This is a handy reference, btw: G-Codes They all do pretty much the same thing. I'm just another hobbyist, but I'm here because I think OpenBuilds Control is the slickest, most user-friendly controller, and it's what I use 99% of the time (I do sometimes use bCNC because of it's height mapping features, but that's not relevant to what you're doing here.). I don't own any OpenBuilds hardware Try again, even without a tool in the spindle to check whether the machine actually moves as expected, or if there is some other problem.
If I'm reading this right you think that using absolute mode means that the machine will always go to the exact co-ordinates in the g-code. Unfortunately our hobby level machines have "open loop" control systems - there is no feedback to tell the controller whether the previous move was successful. If it wasn't, the controller "thinks" it knows where the machine is but it's wrong. If it is losing steps (stalling) the errors will get worse with each move. Alex.
That lightens me up, thank you. The idea with running it without a tool – laid just around the corner.-) so tomorrow there is another testing day.
Yes, this was my assumption. But now I have learnt another thing. Overall: Which area is not that fragile in case of machine-types? For me, I thought, it's hardened metal (the tool) and the stock is wood, not even hard wood. Do I have to go with carving with this kind of a machine, the TTC 450 pro? The alu profiles are quite sturdy but the weak point are the bearing rollers on x and z, specially the x-axis. Two narrow and its not metal. (Here, to be honest, the weak guidance saved probably a few tools as I crashed into the stock).
most of us have been using wheel guided machines for years without problems. They do need adjustment every 6 months or so, and while looseness is obviously wrong, TOO TIGHT is also a problem, the Openbuilds construction videos show the correct tension to put on the wheels. RPM, and stepover = the depth of cut per tooth, remain the same across most machines, the cutter needs to cut and make chips, 5 to 10 thou is usually good, cardide cutters can and should go high RPM , but the big factor is machine stiffness: Got a 4 ton cast iron monster? then you can cut 3" deep in a single pass. Got a belt driven aluminum framed router? Then you can cut about 30 thou deep (but at a high rpm and feedrate, the cutter must make chips not dust). This is ver ymuch like 'HSM' High Speed Machining where the depth of cut is shallow but rpm and feedrates are high, even in titanium
I am dealing with the hardware at the moment, checking the guide blocks on the x and z axis (maybe also y), I have seen that the wheels are very, too close to the threads holding the axis-spindle; there are a kind of two spring-thread-construction holding the axis) AND I am going to upgrade the firmware. With Two Trees it is a bit confusing but they are helpful at the support.
