Feed Rates in Aspire

[steffen707]

I just bought a shopbot desktop, I'm going to be making 3d relief carvings of photos with a roughing pass with a 1/2" end mill and finishing pass with 1/16" ballnose bit.

What should I set the feed and plunge rates at? Where can I find this information in the future, other than from your guys' expertise? Does it matter what wood i'm cutting? This will be done on oak and aspen wood.

Are the feed and plunge rates determined by the Aspire software when you export the toolpaths? Or does the Shopbot Software Suite control that?

[steffen707]

Also, i have no idea what RPM I should be setting things at. How do people learn these things, trial and error?

[scottp55]

jon, THIS helped me a lot!http://www.precisebits.com/tutorials...s_n_speeds.htm

[Brady Watson]

Jon,
I would rough using a 1/4" tool @ MS,2,1 @ 13,000 RPM (@ 216 Hz on VFD if using spindle) and do a 'rough 3D finishing pass' with an 1/8" ball, 25% stepover. I'd crank it up to 18,000 for the 1/16" ball for final finishing (8-12% stepover)- same MS unless you think it needs more or less. Listen to the tool...If it is burning, reduce RPM or increase MS & vice versa. Softer non-plastic materials and smaller dia tools like higher RPM.

Drop your pass depth on the roughing tool to .0625" and do a profile toolpath at least 75% down the total thickness. Carefully observe the 3D toolpath to make sure the toolpath is not falling off the side of the work too deeply. Modify your 3D boundary vector as needed (offset inward etc) until it is contained on TOP of the model. I'll often use carpet tape to hold the material, rough, profile & remove all of the extra scrap. Now only the material that is left will be machined without horrific noise from the tool smacking against the scrap every pass. If it doesn't look right in the 3D toolpath preview in Aspire, it won't look right at the tool...go back & forth adjusting until you are happy with it.

If you don't carefully clear out for a 1/16" finishing tool, you can snap it off pretty easily...and it's usually on the 1st pass. The smaller you make the pass depth on the roughing tool, the more closely it will follow the 3D relief...and the smoother & faster you can cut the finishing TP. Using the methods I describe here I get fantastic quality & have not broken a tool in many years...all the way down to 0.007" diameter

YOU as the programmer/operator must enter in the feedrates as required into Aspire. No default values are necessarily valid - so change the units to inches per second and enter in your own speeds & RPM if you have spindle speed control. Hold your values up against what you may use if you were running a hand held router - then give it a try. You can always change move speeds (MS) on the fly in SB3 to get it to run where you want it to by pausing the tool, and Insert Command, then MS - then the speed you want - then resume to try it out. You can change MS on the front end after Aspire by running the FE command. Just change any MS,xy,z to whatever you want. (e.g. - MS,2,1)

-B

[scottp55]

File that away somewhere safe jon!
"When Brady talks, People...."(How does that go again Obiwan?

[Brady Watson]

"When Brady talks, People....

...mutter something snide under their breath?

Pants go on the same way over in these neck of the woods...

-B

[scottp55]

Actually Oh Great and Mighty One
In a wheelchair it's easier if you do both legs at once

Actually your name and others are usually taken in vain immediately after
"AW SHOOT" "-------- said NOT to do it that way!"
In your "neck of the woods" bet you didn't discover moose tracks by your mailbox this morning
Good tips. Saved for when I eventually get more into 3D.

[khaos]

...In a wheelchair it's easier if you do both legs at once...

LOL Scott!

[Justin G]

Brady,
Your above post has some interesting strategies for 3d cutting. I have had my PRS alpha 96 X 48 for about 6 months now and am starting to feel like I have things dialed in pretty well.

I cut 8 quarter Jatoba wood almost exclusively (it is usually about 1 3/4" but sometimes more) and use a 3/8th" chipbreaker as my roughing tool and 1/4" BN as my finisher.

Instead of running a profile pass in the beginning, I increase the boundary offset of the roughing pass to slightly more than the diameter of the roughing tool. I have found that this give plenty of space for the BN to run without smacking anything and doesnt jame the roughing tool up like a fat person going through subway turnstiles. I set the model in the material in aspire with .15" below it and use screws to hold the wood to the spoil board.

for my F&S roughing, I use 75% step over, and .25" pass depth at 3.1 ips X,y and .75 on the Z. typically run about 9k on my 4hp spindle. I leave a .002 skin on the material.

For my F&S finishing, i use 10% stepover on my 1/4" BN (not sure what that comes to and am too lazy right now to bring up my calculator) with 3.5 ips in both X/Y & Z. spindle is around 8000 rpm. This seems to produce decent size chips and the slower rpm speed allows me to run the machine in my garage without animal control coming by to see why I am killing so many cats.

then I do the sideways onion skin profile thing where I climb cut with tabs and a .005 offset using a 1/4" end mill all the way through the material. I Then copy the toolpath and change the direction to conventional while removing the offset and preserving the tabs.

I have also found that when use the blue trace button in aspire the profile line it produces is too far out and I always offset .0625" inward to as to cut a little bit of the model off but to ensure there is a smooth transition from model top to cut out model side, instead of the ridiculous tell tale "lip" that would be present if the profile toolpath is too far out.

For my average size 23 X 10" artwork, this whole process takes about 3 hours.

I would love some feedback/ opinions on what you think I am doing and/ or how to improve.

Jon I figured the dialogue could help us all, sorry for hijacking your thread.

[Justin G]

Oh also, that was my first post in here ever. This is now my second.