Fusion slotting

How do I remove the ramping in and out and just do a clear stepdown.?? I made my toolpath 6x as long as my hard coded program. I'm very new to fusion.

I am the only one with a machining background. So I hard code everything the owner bought me a Haas and said buy what ever you need. Almost everything is basic drilling and milling paths so I just hardcode it. I've made fixtures and all sorts of stuff so far with no cam software. But I would like to get into more advanced fixturing and such.

I just need to slap to 13/16 slots in .450 material 1.5 inches in and .075 step down. Full WOC. 13/16 endmill. Fusion took a 1:12 second toolpath and turned It into 6 minutes.

I currently work in a glass manufacturer where we do all aluminum extrusions.

I am able to draw in Inventor and AutoCAD.


Sent from my SM-G950U using Tapatalk
https://uploads.tapatalk-cdn.com/201...ffe4d0ba15.jpghttps://uploads.tapatalk-cdn.com/201...4943a9762c.jpg

I think you can uncheck ramping in the operation setup. On my Haas, I would use a smaller end mill, maybe 1/2 or 5/8 inch and do a adaptive clearing pass at full depth, 6000 RPM, 120 IPM, full DOC, about 0.035 step over, aluminum cutting carbide endmill.

Then a final profile clean up of about 0.005. 6000 RPM, 80 IPM, full DOC

To learn Fusion 360, I would recommend https://academy.titansofcnc.com/ a free online course that takes you from 0 to machining parts in a couple of days. Uses Fusion 360 and Haas machines.

I'm not a fan of plunging straight in.
In my program it's using the 'multiple depths' setting that slows it down a lot.
I use 'ramping' but I increase the angle setting and that makes it quicker, still less aggressive than a straight stepdown.

Don't plunge straight in, instead, change the ramp type to helix (IIRC it's the default for adaptive paths anyway) and it will ramp into the guts of the cut in a spiral, then work its way out. You can adjust the thickness of each pass. Using the full depth means even wear on the cutter, faster cutting and a cleaner finish.

Surface finish isn't important where I work guys. Basically it's full send all the time because these are small hidden parts for high rise window assemblies.

I clear the part every step down and take
.075 passes
at 2250 rpm
29 ipm
Hs Cobalt 4 flute .8125 flat

Sounds buttery smooth. Rapid to the other side and start chewing. I was just wondering if fusion could speed this up any more a 4 part cycle is a little over 2 minutes.

I was just trying to eliminate the ramp and have the cutter step of the side of the part half the radius of the tool + .100

Do you think a 1/2 cutter or even a 3/8 cutter could keep up in an adaptive clear with a full WOC 13/16?

The owner is fine with supper agressive cuts and drill cycles. We pay like 2-5 dollars for are TiCn drills some of which I've hit through holes in up to 1/2 material with no peck at almost 5k holes. The 7/16 I've had in there almost 4 months.

and tolerances are basically non existent.

The only time you change a tool is when it's completely shot.

Basically I need fusion to machine more agressive than me but not snap tools off or chip weld them.

I'm looking for a better option at this point the owner has no clue what I do and openly says what your saying is all Greek to me.


Sent from my SM-G950U using Tapatalk

You're only going 0.450 deep, so do it in 1 pass. But use a 3 flute aluminum cutting carbide rougher end mill, and pour on the coolant. I would use a 1/2 or 5/8 end mill and just do 1 profile pass since the tolerance is not important. Max out the spindle speed which I assume is 6000 on your machine. Start at about 120 IPM, and then bump it up until the spindle load is in the 95% range.

Adaptive clearing is a little slower but easier on the tool, but you can bump up the feed to compensate. We would normally run your parts with a 5/8 rougher.

Here is a good video illustrating adaptive clearing and feeds & speeds.

https://www.youtube.com/watch?v=2fuYj4trEGg

I'd prob go:
1. Ramp unchecked,
2. Multiple depths set the same height as your full cut depth,
3. Plunge outside stock.

If you have lots of these to make, why not make some sort of palletized tooling that holds 20-30 parts, and you can be loading one pallet while the other one is being run?

Most efficient production does not always mean taking the last few seconds out of a toolpath. :)

PM

Quote:

---

Originally Posted by precisionmetal

If you have lots of these to make, why not make some sort of palletized tooling that holds 20-30 parts, and you can be loading one pallet while the other one is being run?

Most efficient production does not always mean taking the last few seconds out of a toolpath. :)

PM

---

I was thinking about just taking machine ground blocks and placing them in-between parts. In a Kurt 9" vise extending them across 2 vises. Extending the extrusion length from 6" to to 24" and loading it with around 3 stock lengths walking away from it for 20mn. I would have to pre drill the slots tho or run it with through spindle.

Sent from my SM-G950U using Tapatalk

Maybe pre-drill the blanks on another machine? Quick fixture on a drill press or Bridgeport?

PM

Maybe this will help a little, if you are just doing one at a time for now then probably the easiest strategy to use would be the "Trace" as it will just put the centre of the tool on a line you draw with no offsets, have a look at the images below and let us know if it is close to what you want to do, this plunges off the stock so no loss of time ramping or helixing :D
I didn`t know the exact sizes of your extrusion so what it modeled is a "best guess" and just for demonstration purposes :D
I have also attached the Fusion f3d file in a Zip file for you, just open it and run it in your Fusion, I have no idea of what feeds and speeds you like to run for the extrusions so I just set a spindle speed of 5000rpm and a feed rate of 20in/min and that came out at 57 seconds for the job on the Fusion simulation but that is notoriously inaccurate :D :D
Anyway, if it is of any help to you figuring out how to "get er done" then enjoy :D :D
https://www.cnczone.com/forums/attac...d=430186&stc=1https://www.cnczone.com/forums/attac...d=430188&stc=1Attachment 430190