roughing/finishing technique

[fpworks]

Scott_bob,
Very interesting to hear about this Numeryx setup. I firmly believe a more advanced control would dramatically improve the lifespan of the mechanical components in a Fadal as well. The -88 control is very hard on the machine.

You are correct...there is much tuning required to get accurate parts to run fast. If I wasn't concerned about speed, I could just copy the entire program from the Fadal to our Mazak, but then I wouldn't be taking advantage of our much more expensive machine, which I bought because it can run parts faster.

I will be certain to take a look at the Numeryx system at IMTS this upcoming year. When I bought our Mazak, I quickly saw the deficiency of the Fadal control. Lots of people are worried about "conversational" capability and menu interfaces when purchasing a new machine, but IMO the real advantage of a good control comes with MOTION control. All that other stuff is just user preference.

I would be somewhat concerned with Numeryx's "always on" lookahead feature. Reason being, I've found that adjustability of the lookahead feature is required to find the proper blend of [floor] finish quality, cycle time, and part accuracy between every part. Every part has different requirements, and the aforementioned items are all related by a give and take relationship.

BTW, for those who doubt the practicality of 400+ ipm, here is a video of our Mazak running one of our parts. (BTW, this is a wimpy cut that doesn't remotely challenge the machine) Parameters:
Spindle: 12,000 rpm
Feed: 210-460 ipm (variable by Mastercam highfeed option, AKA "adaptive feedrate")
Tool: 0.375" 2 flute uncoated carbide endmill
Engagement: 40% radial, 0.28" depth
Material: 6061 aluminum

http://www.foreprecisionworks.com/video/MVI_2165.AVI


This following video is facing with a .75" endmill at 460 ipm and 10,000 rpm (would go to 600 ipm, but there are too many tight direction changes and the workholding is questionable...ripped a part out at 525 ipm earlier)

http://www.foreprecisionworks.com/video/MVI_2164.AVI

[krustykrab]

Perhaps my settings, but couldn't download the video.

That sounds like a pretty healthy cut for an endmill that small.

I have a minicut 1" dia. high polish aluminum roughing endmill (interupted cut) that I like to use. Cuts like butter. I can take a 1/2" stepover and 1" d.o.c. with an rpm of about 1800 and feedrates of about 200 ipm. Does that seem good? I don't use a lot of endmills, so I like to learn more from other people. Most of my cnc machining is 3d using indexible high polished carbide cutters.

Anyway, back to your original post. I must have misunderstood your query. I will go back and read it, I apologize for not being more thorough.

ScottBob, I too have heard of Numerix from my Fadal service guy......who I see quite often :/. We did look into it about 5 years ago, I think. Their quote was $35,000 to install the controller and have all of the retrofitting, done.......new drives, scales, etc. To much peanut butter on my toast!

[fpworks]

krustykrab,
No apologies required...we are all guilty of skimming posts as well.

Try saving it to your computer first, then viewing.

Your cutting parameters are healthy, no doubt. I'm not trying to pick, but your machining strategy is old school and there are better and faster ways to handle it, ONLY IF you have a machine that can handle higher feedrates. I'll try to explain:

In that cut, you are removing 100 cubic inches per minute, which is a descent amount of material. BUT, it isn't simply about material removal, because in real world applications, your cut will not always be 100 cubic inches per minute all the time, unless you are cutting straight lines every day.

For instance, I would handle that cut with the following parameters: 1" deep, 0.2 stepover, but feed at 450 ipm, which is relatively conservative. Note that the material removal rate is about 10% less than your cut, but it will cut almost any profiling or pocketing geometry faster. (the effect will be more pronounced with more complex geometry) Please feel free to enter these parameters into your CAM system and see for yourself.

Why? If you were to take the average material removal rate during the cut, it will stay consistently higher. The toolpath has the opportunity to be more efficient with a smaller stepover. (follows geometry more closely AND less air cutting time)

I know this may be difficult to understand at first...it was for me, but this is the sole reason behind high speed machining...faster, lighter cuts produce parts faster than heavier, slower cuts. With the Fadal control, this concept simply doesn't apply...however, keep reading ;-)

This phenomenon is why adaptive feedrate (from your cam system) works so well. (I apologize if you already know how it works, but I'll write here briefly for others) Since your cutter will not always be at your stepover or angular engagement that you specified in your cutting parameters, you will leave quite a bit of time on the table. Adaptive feedrate will post a new feed (sometimes on every line) based on the volumetric removal rate in which your cutter is engaged.

Having said that, and referring back to the video in which I specified 210-460 ipm with a 0.375 endmill...I am cheating, since the stepover is not maintained when the feed is commanded at 460 ipm. The adaptive feedrate makes it so that when the cutter is fully engaged, the feed is 210 ipm. As the stepover decreases (even to air cutting, which is eventual) the feed progresses to 460 ipm.

Since nothing is free, the ability to feed at these higher rates brings forth accuracy problems, and for the control to "prepare" for these [programmed] high speed corners so that it doesn't tear up the machine, and can maintain accuracy. (hence my original question in the post)

To give some further examples...when we started our business, we had a CAM software that was unable to post neither adaptive feedrates nor a high speed toolpath with nice rounded corners. Also, we were also using our Fadal with 6000 rpm max and using old school techniques...heavier, slower cuts.

With our Mazak and higher end CAM software, AND applying the aforementioned techniques, here are the examples of our production improvements:

Part 1: Before=21 minutes, After=5:15
Part 2: Before=35 minutes, After=12 minutes

Granted, 2-3 minutes on each part was also saved in toolchanges, axis acceleration, and rapids. BTW, applying the adaptive feedrate on our Fadal saved ALONE saved four minutes on each part on "Part 2." (not reflected in the above times)