It would be best if you upload your file (file, export).
David
David
Romans 3:23
Etsy shop opened 12/1/17 - CurlyWoodShop
Those errors won't stop the G code from posting. Fusion is notifying you that it was not able to do quite what you told it to, and it is making a correction. I have never seen that error, but best guess is that you tried to set a plunge or start point that is out of the tool path.
Jim Dawson
Sandy, Oregon, USA
Tried just taking a lot of defaults but I would sure like to know what I screwed up.
I did a file export from the MANUFACTURE menu.
When I tried to attach the file I get this
Attachment 419548
Zip the file.
There are limited file extensions allowed to be uploaded!
Regards,
Arie.
zipped file attached
I couldn't open the file, said it wasn't a valid zip file.
David
David
Romans 3:23
Etsy shop opened 12/1/17 - CurlyWoodShop
ok try this one
uugh sorry that one did not have the error tool path in it.
Please take a look at this one.
Also in the previous one it only cut to .475 and the stock thickness is .5. I dont understand why.
Thanks
The reason it's not boring all the way through is because you have Stock To Leave set at 0.02". Turn that off and it goes all the way through. Not sure on the plunge outside of stock message, only had a minute to look.
David
David
Romans 3:23
Etsy shop opened 12/1/17 - CurlyWoodShop
Well, on this last file you uploaded, you are using a the "Pocket" method to bore 4 holes. (there is no machining shows on the slots)
On the 4th tab in the "Pocket" routine you are using, you have "Stock to Leave" checked, and difalkner pointed out that you are leaving .020" stock axially AND radially. Even if you change that, you will probably still get a warning, as there simply is "almost no room to move" inside that 5/16" hole with a 1/4" end mill trying to pocket it.
Those 4 holes should be drilled if at all possible, and if you insist on machining them --grin-- with that .250" end mill, then the correct method is to use the "Bore" strategy. I've added that method as another process, and re-uploaded the file.
OK... uploading another file for you to look at.
I'm making the assumption that you would like to use that 1/4" end mill for most everything, so.... I created a way to cut the slots using 3 different methods:
- "Bore" the ends of the slots
- "Trace" the centerline of the slots, ramping down but staying on the centerline
- "Profile" the outside wall with a finish pass
I also added a sketch with a single circle on it at the end of the one slot I machined, so that I could select the center of that circle as the entry point when doing the Profile pass (i.e. plunge straight down to full depth).
All your feed rates appear way too high to me, so I'd recommend dropping those way back, at least initially.
If nothing else, you can see 3 different methods to cutting a portion of the slots. There are other ways to do it... you could profile and just ramp down along the perimeter, you could "bore" one end and then use adaptive clearing to remove 98% of the material and then just a quick profile pass. Lots of ways to skin the cat! The approach I would probably take would be to set up a 5/16" drill in another holder, and drill one end of each slot, and the 4 holes. Then go back and adaptive clear the slots and run a quick profile pass to clean the outside.
Fire away if you have questions.
PM
Thank you all for the help. Much appreciated.
I will take a look and give it all a try.
It may be perfectly fine in a straight line or a larger profile, but programming 60"/min in something like "boring" a 5/16" hole with a 1/4" end mill might overwhelm your your machine's ability to follow the programmed path.
No way of knowing. You're cutting MDF on ... is it a CNC router table? Not sure what cutter you're using. If you're able to cut 60"/min in a straight line without any issues, then you "might" need to just slow it down a bit for profiling the insides of those slots. That's a tight corner to make if you look at what the centerline of the cutter has to do to make that corner.
I'm sure you have a lot more experience with MDF than I do, so you will have a good "feel" for how fast you can cut it. I'm thinking more about what your machine has to go through to make a tight arc/circle at high feed rates. :-)
PM