[fpworks]

Since this thread has been revitalized, I figured I'd ask. (Let's see this one get hijacked by resonance testing!)

And I know this isn't really high speed machining, but I think it is above the other general machining forums.

In regards to 2D profiling (contouring) in aluminum.

On our little slow Fadal, I typically leaving 0.005" on the walls before taking a finish pass, which works fine in most cases.

However, now that we have our 12,000 rpm Mazak, I typically rough at 350-450 ipm with 0.5" or 0.75" endmills. As you all know, about any machine will try to cut corners at that speed (of even larger arcs), but can be minimized by inducing the high speed look ahead at the compromise of cycle time.

Having said that, what is YOUR technique for roughing/finishing?

1. Do not call the automatic accel/decel and leave more finishing stock
2. Call automatic accel/decel for last roughing pass
3. Something else?

I've been using a combination of the above depending on the feature...can't quite figure out which one I like best. Of course, there are obvious advantages and disadvantages to either technique. Just wanted to get other's opinions of what they found works best.

Justin

[PBMW]

I would think that the turning of a corner at 450ipm would be pretty hard on the machine. Personaly, I use G8's for look ahead and I use them on rough as well as finish moves. I would also think that a contour of any complesity at 450 ipm would be pretty jerky without look ahead
But that's just me.

[fpworks]

I'm sorry, maybe I wasn't being clear about the mode that I'm talking about.

In my experience, G8 doesn't have anything to do with lookahead. The machine will drop feedrate WHILE in the corners, but it doesn't plan ahead by decelerating BEFORE the corner.

I'm talking more in regards to a lookahead mode where the controller will plan in ADVANCE and modify the feedrate as required to follow the programmed path. User parameters are available as modifiers of this mode to find a compromise between accuracy and speed.

With the Mazak, the mode is called with a G61.1 or G5. I think Fanuc controls use a G5 also. Our Fadal doesn't have such a mode.

In the lookahead mode, you can FEEL it working harder to follow the contour if you put your hand on the machine. This is why I use a G64 mode for roughing. In normal cutting mode (G64) the motion control is smoother, but the controller will cut corners to maintain highest possible feedrate, often to the point of violating the final part boundaries. (it does actually drops the feedrate in the corners, but it doesn't "plan ahead" by decelerating BEFORE taking a tight corner)

In regards to machine jerkiness, of course, our Fadal would rip itself apart at 450 ipm, but the Mazak is silky smooth at those programmed speeds, especially in G64. It isn't a problem.

[Caprirs]

On my Mitsubishi controlled mills, I have the G61.1 and G5 as separate commands. On the Mitsubishi, both can be used simultaneously.

G5 is the look ahead for maintaining constant feedrate over a 3d surface such as mold cavities made up of zillions of tiny G1 moves. It is actived by G5 P1 and deactivated by G5 P0.

G61.1 is considered high precision mode where feedrate is sacrificed to maintain accurate position. There is a parameter which adjusts how far ahead of a corner the machine slows down in order to maintain an accurate path. The setting is time based so it has to be adjusted according to the feedrate that will be used. I don't know how that parameter is accessed on the Mazak.

In answer to your original question, I tend to leave more stock on the part so I can rough faster and not use the G61.1 until the finish pass. My machine will do as you describe where it starts turning the corner too early at higher feeds resulting in odd shaped corners. If I leave .010" for a finish pass, I get good results.

[fpworks]

Caprirs,
Sounds like the controls are nearly identical. The Mazak uses a Mitsubishi Meldas control also.

Thanks for sharing your technique. Just out of curiosity, how is your contour accuracy affected around corners when the finishing stock is more/less than the rest of the part?

I've had some issues with sharp inside corners, unless I use G61.1 on the pre-finishing pass.

[krustykrab]

I have been cutting aluminum for quite a few years, so I have a few questions:

1) You haven't really identified which machine you would like to optimize.

2) What kind of controller is on the Fadal? (if this is the machine that you are concerned with)

3) What does the part look like? This is integral to the method of machining.

4) 2d profiling and "contouring" are almost the opposite of each other. (again lets see what you wish to cut)

5) Is roughing at .005" per side? Or is there a semi stage involved?

6) what kind of aluminum?

IMHO, if you were planning to rough on any machine to .005" per side, you had better use all of the look ahead features available to the cnc machine!

Also, you have to consider how much you wish to mash up your bread-and-butter......meaning, if you run the machine at 4-500ipm and its bouncing around like a jackhammer........what does that benefit? Forget about tolerances when the thrust bearings are flattened out. (aka fadal cnc88hs syndrome)

In my experience, cutting 2d or 3d, if you semi to a thickness of .011" per side at maximum machine feedrate using contour contol, finishing thereafter at approx. 100ipm, will leave no stock...as long as cutters are sharp and contour control has been activated.
But that's pretty general...like I said, let us see what it is you are trying to machine.

Hope I can be of some help.......and maybe learn something here at the same time.

Cheers!

[Caprirs]

If I'm machining an outside profile like a square, I cannot go around the corner faster than 75ipm on the finish pass without using the G61.1 command. Without it, the machine starts the corner too soon and leaves something visually ugly.

For roughing, I think i get as much tool deflection from the cutter pressure as I do from machine error from high feed rate. Thus, I can't really rough .005" from finish dimension even if the machine would hold position at high feeds. I have not tried roughing using the G61.1 because it's faster to leave it off and leave more material to finish.

[krustykrab]

try separating the square into 4 passes each linked with horizonal arcs.

[fpworks]

krustykrab,
To respectively answer your questions:
1. Mazak (identified in the first post)

2. N/A (300+ ipm feeds are not practical on a Fadal)

3. N/A, this is a generic question in regards to a technique, without respect to any particular part.

4. Symantics...in the original post, I specified 2D profiling (contouring)...sorry, didn't mean to be confusing. (profiling and countouring are used synonymously in our shop, and in Mastercam) The word "countouring" does not necessarily mean 3D contouring.

5. 0.005" is in reference to the finishing stock. This is the material remaining after roughing, that is to be removed for the finishing pass.

6. N/A...this is generic. High feed rates can be achieved with any type aluminum.

Don't worry about bouncing or jackhammering. This machine contours more smooth at 400 ipm than the Fadal can at 100 ipm, but this smoothness is at the sacrifice of cutting corners and violating part boundaries, hence the reason of this thread.

This thread has nothing to do with any particular part...just general technique. The parameters associated with the lookahead mode are adjustable for the application.






Caprirs,
It sounds like you have your accel/decel gradients set much lower than our machine. If you don't mind me asking, what does your G61.1 accel/decel gradient? Do you use the additional "K" value on the G61.1 line? I modified ours quite a bit from the factory settings because the factory settings compromised too much accuracy. It is now currently set at 0.1G if I remember correctly. (from the factory, it was 0.5G)

I regards to the finishing stock question, I need to clarify.
When I use G61.1 for a pre-finishing pass, I (obviously) get more consistent finishing stock for the final finishing pass. I've found the if I don't use G61.1 for pre-finishing an inside corner, much more material is left on the inside of the corner, which influences the accuracy of the final finishing pass. Any problems with this?

[Caprirs]

As far as I know, my Mitsubishi M3 controls have no provision for an additional "K" value on the G61.1 line. That might be something specific to the Mazak software. There is nothing in the Mitsubishi manual about it so I've never tried.

The only value I have adjusted is the variable in the machine parameters, base spec, page 4, G1btL. I normally have this set to 100 with good results.

For your pre-finishing pass, you can use the G61.1 to ensure that your tool is getting as much material from the corner as programmed. Another option is to use the automatic corner override G62. This feature identifies inside corners and slows the feedrate on approach to the corner to reduce the loading the tool experiences. It cannot be used simultaneously with G61.1. Cutter comp must be turned on for it to work, but you can put a nominal value in for the tool radius like .0001". When the tool approaches a corner, it drops the feedrate to the %override specified in user parameter, setup, #4, #5, & #6.

[Scott_bob]

I am thoughly enjoying this discussion...

This is really crucial for the Fanuc and apparantly the Mazak guys to fully understand. And for those poor souls who still have Fadal controls well, they cannot understand what you are talking about when you say your CNC is silky smooth at "programmed" feed rates of 400 - 500 Ipm.

Also, it is crucial for CNC users to understand that without buying those expensive options that your machine tool builder is selling, you cannot understand what is being said above, any more than the Fadal users (who don't have these capabilities). Without these upgrades to your Fanuc or apparantly Mazak controlled CNC cannot perform at these high "programmed" feed rates...

This is a fact. Evidence: see above...

I also share the frustration "above" that it is too much trial and error to get both accuracy and high performance feed rates out of a Fanuc.

I have witnessed, and handled with my own hands, and trained others to use this control called the Numeryx. I have never seen better motion control. If you have a passion for your machining, go see one in action.
They are out there. If you want 2nd to none performance, why not take a trip. Go to Detroit yourself, or one of the high speed machining shows and get a demo of this control.

By the way, the feed rates you mention above where possible on the Fadal we retrofitted with the Numeryx and the ballscrew thrust bearings saw less jerking than they did with the Fadal MP32. This machine could hold accuracy of +/-.001 at very high feed rates as long as you have already taken care of tool deflection by leaving .005 or .010 for the finish pass. As long as you are climb milling your deflection will be away from your 2D feature, and in 3D there are no undershoots or overshoots to worry about. It's all automatic, no G61.1 or G5 or any other modifers either. It's just accurate all the time. Set one high feed rate your tool can handle, don't cut too deep for that tool and let it go. This is no exageration...

Good discussion on this subject!

[hsmexpert]

The best the Fadal can do and maintain part integrity is about 40 inches/min.
look at www.vibrafree.com they have a bunch of actual parts with cut times, you will see some excellent results with real high speed hard milling.

[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)