I've made a few of these guitar trays but haven't run into this. The fusion file and toolpaths seem correct but when I did the first contour it's like everything shifted left just slightly. The stock is extremely secure so I don't think it's that. I'm questioning when I went from an adaptive clearing using a 6.35mm bit and collet then going to a 3.175 bit and collet. I probed everything correctly, hard to mess that up. The picture shows the bevel just after the contour path. I had a feeling the bevel would go a miss considering the previous toolpath messed up. Any ideas?
Sure you remembered to change the Bit Diameter field on the probe wizard to the new smaller bit before probing with it after the toolchange?
You only needed to re-probe Z after a tool change. X and Y are set at the centre of the bit, so you don't need to to re-probe those for a different diameter bit. Alex.
Thanks for the responses. I'm 99.9% certain I changed the bit diameter when re-probing from the 6.35 to 3.175. Good to know I don't have to re-probe XY for tool changes. I thought if the diameter changed then the XY did as well. I thought I may have chosen the wrong tool in F360 but that checks out as well. If I didn't know any better I'd say something happened in the probing. I'll try to not reprobe on the next round. Somewhat related, if you look at the pictures you can see where the contour path is a little deeper in Z than the adaptive. In fusion the adaptive toolpath has .5mm of Radial stock which I thought was on the sides, Axial would be Z. I probed all from the bed with the OB probe plate. Not sure what happened there either.
Rhett. I originally wrote this - "I think the CAM program is executing as specified (see trial image attached). The engraving tool is centering 1mm inboard of the material on the specified path. I haven't tried it, but I think you need to specify a tool capable of chamfering instead of an engraving tool with 2D chamfer as the operation." I have since found the problem was the direction of the path for the chamfer. Edit the path direction by clicking on the arrow when the Geometry tab is selected for the operation.
Thanks, Rob. I was just responding with another perfect example of what's happening. I've used that bit (60deg vbit) for chamfering in the past and I haven't had issues like this. It's also offsetting with the 3.175 endmill. I just re-engraved the name with the same bit I used for the first engrave. I tried a resin enlay that failed so I went to 'erase' it. I got the same offset to the left as I did with the endmill stated above. I did this today after starting the machine, re-homing and paying special attention to the probing process. Seeing Rob's example shows something isn't programmed right but why would it happen with the 3.175 bit as well? The image shows the blue resin inlayed and the new (same) engrave I did to erase it. It's offset to the left. I appreciate everyone's help. It's frustrating making a mistake when you've spent so much time on the stock.
That worked, Rob. I changed the offset width a bit but the simulation now shows the tip of the bit just inside the path, not directly inline. I always thought that red arrow indicated left milling or conventional. Do you think this would cause the issue with the 3.175 endmill contour op?
Just tried with the 3.175 contour path and when I change the red arrow direction it mills out a lot more material than the other direction in the simulation. It still mills the entire thing with both scenerios vs. the real world example where everything is offset. I think I'm confusing myself
It sounds like you might be changing direction on the wrong operation. You need to change the direction only on the chamfer operation, not on an adaptive clearing or finishing contour operation.
I've never clicked that red arrow on anything. You showed it needs to be done on chamfering, thank you. Does that red arrow indicate right vs. conventional milling? That I have changed. EDIT: Simulation tests show the red arrow changes based on 'right' or left milling. Contour op calls it sideways compensation and an adaptive clearing calls it climb and conventional.
I think you know as much as I do about chamfering at this point. This isn't an operation I have needed to use yet. FWIW, I can make some other suggestions having seen your Fusion file for this. 5mm DOC seems a bit big for these machines with those tools Chip load seems low (only .028mm) so surface speed is low for a wood cut. Perhaps this is how you get away with the large DOC but it means you might be creating more dust than wood chips. You modelled a solid block and then did an extruded cut to shape the outside. This is a redundant step. Just extrude the contour shape you want and specify appropriately sized stock material in the CAM step. The sharp interior contours require sudden large tool loads for the finish internal contour operation - particularly for the smaller milling cutter where the larger cutter was unable to clear material. Look for strategies (adaptive if possible) to abate this. No tabs to hold the cut part after the outer contour is cut. You can often get away with this depending on the hold down method but sometimes with clamped stock the freed material can be problematic.
Arrows during setup on single countours- Chamfer, Contour, maybe Trace, etc determine which side of the line (or inside/outside of closed vectors) it's using for calculations. Should show immediately if it's wrong in the green simulated model when you select the operation.
Sounds like this explains what happened. First adaptive path then contour. I must have switched the two. I appreciate the input.
Thank you for the feedback, Rob. I have a love hate relationship with Fusion but I'm still learning. I need to go back to the basics with surface speed etc.. Can you please elaborate on your 5th bullet point? In the project for this thread I was thinking an adaptive to clear the pocket, then a contour to clean up the edges. Maybe use adaptive for all the 'pocket' operations? Thanks again
You refer to the 5th bullet but you seem to be talking about the 4th. Assuming the 4th, you could use another short 2D Adaptive operation with Stock to Leave with the 1/8" bit with the "Rest Machining" option for the previous 1/4" bit. This should clear out only the areas in sharp corners not reached by the previous 2D Adaptive operation with 1/4" bit. Then the next 2D profile cleanup pass as you have it now would be less irregular.
