Efficient Hole Machining?

[LibertyMachine]

Challenge: Most efficient hole machining strategy, AS WELL as smallest g-code possible.

Details: I've got a part to make that has several holes. It's only one part, so it "really doesn't matter" how efficient it is. However, I desire to properly apply all that Fusion has to offer and make better use of strategies as work requires. Perhaps the next job that lands on my desk has many more holes and will be in my machine for several weeks. Of course then, every EXTRA second spent machining costs $$$, as well as the demands on the machine control processing a large amount of code. I'd rather learn things now, instead of when they REALLY matter

I've attached a couple different strategies that present themselves as "the solution", but in my estimation, they both fall short...

Feature is a .650 dia C'bore, .500" deep. Hole is predrilled .437". Goal would be to plunge down and sprial out. Endmill is .375"

First up: Circular tool path.

Pro's: Very short toolpath, about 15 lines.

Con's: Z rapid to top of part between cuts, wasted time.

Con's: Leaving the cut between passes, wasted time

Con's: Lead back to center between cuts is also wasting time. 

The second path is 2D pocket (I had almost identical results with adaptive)

Pro's: Tool stays in cut in what appears to be a constant spiral out, which is perfect.

Con's: Code is about 150 lines long for one hole. I've tweaked all the smoothing and tolerance setting with little improvement. Seems to be an arc, then a very small G01 move, another arc, another G01, ad nauseum

Con's: Tool spirals from center. If there is a large pilot hole, this would be wasted time.

Ideally, I'd like to find something similar to the 2D pocket path, without the file size. I know that CAM generated code will always be larger than what one could produce with a pen and paper. However, I know of 2 other CAM packages that have hole strategies that accomplish exactly what I'm looking for (MasterCam and Esprit). It's just a short string of G3's with ever-increasing X positive and negative values with an increasing "I" value

Quick Edit: Furthermore, is there a way to "force" the CAM to produce toolpath that enters at a specific angle, relative to the part? Ideally, I'd like to enter into the part at a full 90 degrees (3 o'clock position), further reducing the code and making it more readily understood by the machinist. Code is easier understood when it is simply: G3 I-.125 instead of G3 I.031 J-.0543

[Anonymous]

@LibertyMachine, There are so many answers to this question it is practically unanswerable.  So, I'll make a few points instead of try to answer your question.

At the level of efficiency you are striving for, having refered to the feed time back to the center of the hole as waste, I would be inclined to do the most efficient of all and use a .650 diameter endmill to plunge the counterbore.  Afterall, the scenario where this would matter would clearly justify the cost of the custom tool.  We're being real world right?  One line of code per hole is pretty lean and very easy to understand.

How do you define efficient?  What are the metrics by which you measure it?  Time?  Lines of code?  Ease of interpretation?  The 2D Bore operation is quite simple, especially if tweaked.  You can disable all the leads and use "lead to center" to get rid of hard to interpret code.  Finish passes can be free from retraction to center also.  But, we're still talking abour 15-20 lines of code per hole.  This path would get my vote personally.

I program a LOT of one-off work, and a fair ammount of low to medium production.  I do very little to no high volume production programming, so optimization at this level is not my specialty.  Having said that I understand the requirements of high volume production and I know these things matter.

One last thought to expand on that last statement, I can't imagine a shop so concerned about high level optimization would be concerned about being able to easily read the code or how many lines of code are required for the operation...within reason.  The highest speed, best time-optimized interpolation paths are not typically comprised of 2D lines and arcs.  They are complex computer generated paths (technically many many lines and arcs I guess) tuned to remove as much material as possible in as little time as possible, and with as little tool wear as possible.  That is the ultimate goal for high production.  Invest in high speed machinery with high RPMs, fast processors, sufficient look-ahead, and lots of memory.  Invest in high speed capable software to get the most from that equipment, and harness what technology has to offer us.

HSM is the best thing to happen to the machining industry in years, and the fact that it is happening everywhere you look these days is exciting.  Embrace it.  That is just my opinion.  There is no right or wrong answer to your question.

[daniel_lyall]

one of the first things I do is get the correct cutter for the matterial and the biggest posable to fit in the hole. you would be surprised how much a diffrences it can make, you work out the max`s chip load for the cutter what gives you max depth and width of cut if it`s pery drilled you dont need lead in plunge down and cut.

ask the machinest who the code is for what he thinks the machine could do if that person is not a buttion pusher that is.

I cut manly wood but it`s all realtive, it`s pucker factor when you sprial a 1/2 inch cutter down 25 mm and cut with a 50% step over and nothing break`s that`s the power of HSM there.

if I tryed the samething with V Carve pro it would set the machine on fire it`s happened twice not by me 

A code that would take 1 hour to do in V carve pro, fusion cam can do it in 20 min`s

[LibertyMachine]

@Anonymous @daniel_lyall, 

Without giving an exhaustive rundown of my 18 year machining resume, suffice it to say that while I know I am not in the top 1% of my field, I would say that I am quite far from being a button pusher.

That being said:

HSM (High Speed Machining): I love it. The shop I've been working at for the last 7 years uses it extensively. That being said: It has it's applications, and it is NOT the solution for every material removal process, nor is it the solution for every material to be cut, OR every milling machine. New modern machines take very well to HSM. They have fast servos and fast processors that can read ahead several hundred lines and make for a very smooth toolpath, even though it is comprised of several hundred or thousands of lines. On the other hand, dated equipment does quite poorly, in my experience. By dated, I mean mid-80's into mid 90's entry level machinery. It wasn't until the late 90's that "most" CNC controls were able to handle code that was quite large, comprised of many small moves. Those of us with dated equipment (my home shop) still need to be efficient in what we do, considering profit margins, time spent at the machine etc. 

Readability of program: Once a program is up and running, cranking out good parts, who cares what the code looks like, right? If it works and the cycle time is acceptable, then that's really all that matters. I understand this attittude and fully agree with it. The flip side of that statement is with the person setting up the job. I don't know about you, but I'm not likely to touch off my tools and just "go for it". I try, if at all possible, to at least run the tools above the part, make sure it doesn't do anything stupid. Some of the projects I've worked on over the years have been in costly materials, no extra pieces, tight tolerances. Perfect recipe for stress on the machinist and a contributing factor to my hair loss. Being able to find a spot in the program where you want to MANUALLY add an extra pass, maybe take depths of cuts, etc, all contribute to the concept of making a program easy(er) to understand, should the machinist need to fiddle around in it. Having HSM at every opportunity removes that ability from the machinist. Again, HSM is good, when applied where it is needed.

Plunging straight in and tool selection: If surface finish, location and size are relatively irrelevant factors, then yes, plunging in with the proper size works fine. However, if those requirements are there, then you really should interpolate the hole. In regards to tool size: If I was constantly working in a soft material such as plastic (or wood), then yes, going for the absolute largest tool that would fit into my pre-drilled hole would be the correct answer. If you try that in Inconel, Titanium, Monel 500, or any other "exotic" material, let's just say, you are going to be in for a rough time...

Ideally, what I would like to find is something like a cross between the standard circular toolpath and the 2D adaptive. Start at center (If preferred), specify clearance size to allow for high feed movement so you don't waste time cutting air, spiral out with simple arcs to finish size. If you are familiar with Yasnac controls, this would basically be a long hand verion of there G13.

Toolpath with plot out very similar to adaptive (constant spiral that looks like the scroll in a 3-jaw lathe chuck), compact file size to allow running in older equipment.

[daniel_lyall]

so you have a good grounding then so you do know what`s what. ( I dont know what you know) having the correct tool maxing the chip load per material is half of it, the rest is what the machine can handle and haveing the correct cut type, this part is experinces with a machine only you can answer that.

it`s the same with me I know what the max cutting i can do on each type of wood I cut and half the time I use the tool path what is suted to what need`s to be done most of the time it`s not the recomend cut type but is the one that work the best.

I also cut aluminum I just get the correct cutter for the grade it is then I can run it at it`s limit becouse I know it`s not going to weld I just use air blast with a bit of water driping into the air stream. this is just to save money and time it`s only $10 a mm for the cutter`s but they can do 30 hours, a HSS tool may do 2 hours 

[kb9ydn · Accepted solution]

2D adaptive will do everything you ask except for entering at a specific angle.  And with the right smoothing settings you can get some pretty compact code.  Try posting this and see what you get.

C|

[LibertyMachine · Accepted solution]

@kb9ydn,

Thank you. Apparently, there was one more pass and smoothing tolerance combination that I hadn't tried. Turns out, if you give it more tolerance, it will make more code. Hmm, something to keep in mind. I had originally been trying a .002" pass tolerance and a .005" smoothing tolerance. That gave me 150 lines for one hole. With a .0005" pass and a .002" on the smoothing, it was under 20 lines. Good to know, thank you!

[kb9ydn]

Yeah, the smoothing and tolerance settings are funny sometimes.  Though I'm a bit surprised that 0.002" and 0.005" made such large code.  Most of the time I use 0.0002" for tolerance and 0.001" for smoothing; and that gives pretty good results.  But sometimes I bump them up if I'm really memory constrained, like on my old Bridgeport.

Anyway, I'm glad it worked for you.

C|