high speed machining tip...

Maybe folks know this. I knew it, but never really thought about it till I seen the effects of it.
In every cam system Iv'e been on there's a spot to add fillets to the
toolpath. I used it when I wire edm'd dies, they usually put a .005 radius on all corners, so I would add it there. But it's really for high feed milling. By putting a value of .0005 in there, corners will not dwell at all. Something about an arc, it's real smooth. Just by adding a .0005 arc in all corners when cutting electrodes, all cutter squealing went away, dead quiet. I havn't tried it, but I wonder if a value of .0002 will work. Maybe it just needs the g02 posted out to keep it from dwelling, or whatever it does in corners.
So lets say your roughing out a pocket, a shape, an electrode, etc...drop something in there, it will extend your cutter life and run nice and smooth in corners.
Just trying to post something on topic, it's not easy.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Q: Whats the quickest around a sharp corner? A: through a radius
--
BB's #95
Help provided
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On 2/26/2010 2:37 PM, vinny wrote:

It has even more uses:
If you are using cutter comp, and driving say a sharp cornered pocket wall to wall, adding a small value ensures the tool will comp equally in the corners as well. Imagine a 1" em reground to say .970. If you don't don't use it, the tool cuts an additional .015 in the corner.
Another use (at least in NX): Most airframe machining requires +.030 then net radial stepover on profile milling before the next step down. Problem is in Seqmill if your tool radius is greater than the difference of the the corner, the processor will bomb out (Seems the corners are always like .390 rad and the tool is always .750...). So I drive wall to wall (don't select the corners) then use a .015 Drive Radius at all the corners. Works pretty well. Note the newer Multi-axis Contour Profile does not have that limitation.
And finally like you said, use it when driving highspeed. Usually use .100r for a 1.25 endmill and say .030 for smaller. There is also coner slowdown that I may or may not use as well.
-- Bill
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
On 2/26/2010 3:25 PM, BillT wrote:

Meant to say "if your corners are the same radius as your tool..." (pretty hard to drive a sharp corner).
-- Bill
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Mastercam has corner slowdown, but you can slow it down over a distance. Most advanced corner gimmic iv'e ever seen, and some guy wrote it as an addon, a chook. Kindof a macro.
And it also has a gforce you can type in for any machine. It allows you to tweak in the corner rounding of your mill. Keep increasing it till your machine bangs, then slightly back off. that setting becomes modal for that machine.
I have to say, mastercams high speed control beats UG's. That was a hard thing to type.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Hey Vin, you been away from NX for a while or didn't look???
Remember the options even in the simple Planer Mill?
Path Shape in Corners? Smoothing, Radius, Stepover limit...
Feed Adjusments on Arcs? Min/Max Compensation Factor...
Feed Slowdown in Corners? Tool Dia percent, Slowdown Percent, Number of steps, Min/Max Corner Angle... (and you can base it on the previous tool)
All off those items dictate what outcome you have for "highspeed" milling.

See the above items...

I'll give you a pass since UG (NX) has never created an operation with words like "Highspeed". It's just toolpath control relevant for the current conditions. Those tools have been in NX for a long time. I mean think about the term Highspeed... it's like Heavy Duty (or Hunky Dori). <g> -- Bill
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Hey Vin, you been away from NX for a while or didn't look???
Remember the options even in the simple Planer Mill?
Path Shape in Corners? Smoothing, Radius, Stepover limit...
Feed Adjusments on Arcs? Min/Max Compensation Factor...
Feed Slowdown in Corners? Tool Dia percent, Slowdown Percent, Number of steps, Min/Max Corner Angle... (and you can base it on the previous tool)
All off those items dictate what outcome you have for "highspeed" milling.

See the above items...

I'll give you a pass since UG (NX) has never created an operation with words like "Highspeed". It's just toolpath control relevant for the current conditions. Those tools have been in NX for a long time. I mean think about the term Highspeed... it's like Heavy Duty (or Hunky Dori). <g> *****
I didn't see all those options, like slowdown percent. I was on nx5?
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
vinny wrote:

There's lots of other uses, too.
Years ago, I was doing some service work on a machine in a customer's shop. The next machine over was a lathe, running some little parts out of nasty material with a .001 tolerance on an OD, and a minimum corner break where the OD met a face. The guy running the machine was new. The cell leader, as he gave the setup to the operator for production, told him that the OD had to be right, and he needed to check every part till they found out how the tools would last.
As I worked, I could see that the operator checked the first few parts; but then got lazy. Pretty soon he was running a dozen parts at a time (short cycle time) between checks. The cell leader came to check on the job, looked at the parts on the bench, and got a worried look on his face. When the operator next opened the door for load/unload, the cell leader stepped up to the machine, looked around inside, and then started sniffing the coolant mist. Then he wiped a finger across the tailstock ways, and then touched it to his tongue, tasting the coolant. "These parts are oversize!" he said to the operator. "I told you to 100% them!"
The operator looked at the cell leader like he was crazy. "I've BEEN checking the parts," he said. "They're fine."
"They're oversize", said the cell leader. "I can taste it. Go back through the parts you've made and check them all before you run anything else." Then he walked away.
The operator was now certain that the cell leader was nuts. But he picked up the last part in the tray on the bench and checked it. Then he quickly put it down and checked another, then another, his face starting to look both amazed and panicked. He had to check back through eight or ten parts before he found one that wasn't oversize. Then he just stood there for a moment, clearly confused, looking back and forth helplessly between the parts on the bench, the machine, and the general direction where the cell leader had walked away.
What the cell leader had actually done was put a .001 radius on the corner where the face met the critical OD. And when the tip of the tool started to wear, that radius disappeared. Small as it was, it was easy to tell the difference between that radius and a sharp corner, even from several feet away. When the cell leader saw the sharp edged parts he knew exactly what was going on.
The sniffing and tasting, however, were pure genius. I'll guarantee that operator followed EVERY instruction for a long, long time.
KG
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

pure BS...I can smell it from here in the UK.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

Do you smell that? That smell........... that BS smell........ smells like......... victory.
--
BB=92s #95 (modified)
Help provided
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Do you smell that? That smell........... that BS smell........ smells like......... victory.
--
BBs #95 (modified)
Help provided
  Click to see the full signature.
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload
wrote:

wait a minute, The Brit's celebrated on july5th? for what? Our independence? I think my history needs updating.
-- BB's #116 Home of the brave And land of the free But not if you crave An SUV
Gil Member of ==American Toolmakers= using the "old world" ways with yesterdays technology building Tomorrows Dreams
Add pictures here
<% if( /^image/.test(type) ){ %>
<% } %>
<%-name%>
Add image file
Upload

Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here. All logos and trade names are the property of their respective owners.