I’m hoping someone here can help me determine what is going on with my parts that I try to cutout from Fusion 360 generated G code imported through Easel. First a little history of what I have done:
- I have adjusted my pots using the video from RobertA_Rieke (thanks for the awesome video)
- I have also done the calibration test from RobertA_Rieke (thanks again for awesome procedures and the file)
- Based on the calibration test I have made the slight adjustments to calibrate the stepper motors based on the video from RobertA_Rieke (thanks again!)
- I ran the test file again the dimensions were within 3 mils which I was pleased with.
Dimensions for items cutout from Easel have been within 3 to 5 mils of shapes created within Easel. Since then I made a relatively simple piece in Autodesk Fusion 360. The part I was trying to create was 1.7" x 3". After I cutout the part, the part was 1.74" x 3.04". I also did a few other shapes using different methods of machining (2D contour, 3D adaptive clearing) and got the same results, being 0.04" too large. I verified that I did not have Fusion 360 set up to leave material for rough cuts. I also matched the 1/8 flat end mill in Autodesk Fusion 360 with the 1/8 end mill in my router. I measured my end mill as well and it is exactly 1/8".
recttest.nc (6.7 KB)
I have attached my G-code file just to show what I have. Any suggestions where I am going wrong?
I have the same issue with anything done in easel .04. I dont think it is the machine because all software i have used the measurements are spot on i just assumed it was a part of easel and make adjustments to account for the .04.
I think Fusion 360 has an option to leave X amount of stock.
Make sure this setting is turned off.
I saw that and it was set to “0”
I previewed the NC file in ChiliPeppr…
It calculated the tool path to be 1.98 x 3.13.
Taking into a .125" bit, that is 1.855 x 3.005.
So one direction seems fine, but not sure about the other.
Maybe double check the model?
The example you posted only has 1 pass around the stock.
How thick is your stock you are milling?
Fusion 360 has a multiple passes option and that should be turned on for best results.
I have no other ideas besides machine deflection.
The material is 1/16 thick ABS. I have tried a few passes as well with the same results. I have checked the model multiple times and it shows 3.0 x 1.7.
Deflection has not been an issue with anything I have milled using Easel (materials and milling location were the same between Easel and Fusion 360). I have also stiffened the gantry using 3/16 aluminum T extrusion and the Y axis rails are stiffened as well.
It is always a possibility when using different CAM packages;
Speeds and Feed rates, plunging vs ramping, climb vs conventional, etc…
One last suggestion,reduce the distance between the stock and the bottom of your spindle; Raise the mill into the collet or use as short of an end mill as possible.
Or maybe it is all Fusion 360’s fault.
If you find your issue be sure to let the community know. It will be helpful for someone someday.
I have been trying to keep both consistent as well (using 35 in/min feed speed and 15 in/min plunge), but I am still learning the other parameters so yes, there is a possibility that something was different. I’ll be doing a few more tests over the weekend to see if I can figure out what is causing the differences. Thanks for the suggestions and I’ll report back what I find out.
I’ve done a few more test cuts using hardboard with a 1/8" flat end mill pushed up into the collet as far as possible.
When I cutout a few test pieces (varying in size from 4-10 inches in both the x and y directions) using g-code generated by Fusion 360 and imported by Easel, my outside dimensions were too large. I dialed in the stepper motors in the advanced setting of Easel so I was within 0.004" in the x and y directions. As another test I cutout a test piece with a few large holes (4", 3", and 2"). The external dimensions of the piece were within 0.004" again, but the holes were 3.95", 2.968", and 1.975".
It almost appears that the bit size is off. I did verify that I input the correct bit diameter of 1/8" in Fusion 360, and I also verified that my actual bit size is exactly 0.125". I have also turned off any settings within Fusion 360 to leave stock. So it that shouldn’t be the issue.
Anyone ever run into this? I may just give they guys at Inventables a call tomorrow to see what their thoughts are as well.
I did a few more test pieces this afternoon and was playing around with finish cuts. Finish cuts got me a little closer, but my dimensions were still off. After doing a little more searching on the internet I ran across this post on the Autodesk forum:
The default for Autodesk Fusion 360 in the CAM function, Passes, Sideways Compensation option is the “mill climbing” which is what I was using (and which is what JeremyJohnstone mentioned above but I didn’t understand what he meant until seeing the post, I’m such a newbie). I should have been using the “conventional” setting since our machines are considered a “less rigid machine”.
So to sum up my rambling, these two things fixed my issue:
- Having a finish pass.
- Changing the Sideways Compensation option in Fusion 360 to “conventional”
Thanks JeremyJohnstone for the help!!
Thank you for this I was going nuts. I have a shapeoko XXL that I am trying to use _reliably_with fusion 360. I don’t get why the default value of climb milling would result in more than the radius of the cutter compensation… I switched to conventional and added a finish pass (actually you have to select 2 finish passes for Fusion to do one(!) With a stepover of 0.5mm and everything is coming out accurately. The cut finish seems better too. So thanks again. Yay forums!
Summary: if you use default climb milling and computer compensation all your features will be oversize by about 1.5mm. If you use conventional milling and computer compensation with the same tool and do a finish pass everything is accurate.
Box joints don’t work well when every hole is 1.5mm too small.