What's new
What's new

Harvey Performance Company (Helical) didn't like my post...I'm SOOO bummed out!

I worked for a company that posted manufacturing related content and ppl would comment on things....typically me and my co workers were not allowed to reply. Amongst ourselves we figured that the "keyboard cowboys" were looking for an argument because there was no down side for them. One guy in particular (yes, he is here on PM) would complain about things and we figured he was just venting because his boss or wife rode him pretty hard so he was trying to vent his frustrations online.
I am not accusing you of that.
Just saying, legit criticism and / or questions can get lost amongst the mindless drivel that is the internet.

Absolutely. I joined a few Facebook machining groups for the secondhand sale stuff. Lots of mindless drivel in the comments... I generally just ignore it and move on. I've gotten to that stage where it's just not worth the time to me. I follow this apt recommendation: Never argue with an idiot - they'll just drag you down to their level and beat you with experience.
 
Have you ever worked in a machine shop or toolroom. Marcus was very polite. The online video is the equivalent of the sales rep turning up with a crap product.
Accusing someone of cheating is likely to draw a large response, especially if it's true. My advice is tactical.
 
That puny mill and end mill would never make it down here in oilfield country machining. Get some real tooling and beefy mill and cut that down to three minutes max to mill out!:cool: Using a manual mill, too!
 
Have succesfully used that style of endmill in pocketing operations in tougher/harder steel when pre drilling a hole is impractical. We use alot of multi flute endmills for machining harder materials...multi flute endmills are a poor choice for ramping in to a pocket. This style of tool is a legit alternative to retooling a machine that has dedicated tooling just for an occasional job. It can be the right tool for the right application.....but not for every application. I have also used them to create a "start hole" and then go into that start hole and create the rest of the pocket with a bottom up style tool path.......its just an alternative way of looking at the job.
Case in point....how to put a start hole in a pocket with the following....material is 40 ish Rc....machine has dedicated (mostly) tooling....machine uses MQL lube.....this tool resolves the issue. Sure a carbide drill with coolant would be quicker....but the machine has no coolant in it because 97% of the work in it uses air or MQL.
BTW....they work good to flatten out a drill point when you can use a drill prior to roughing and they can be extended out of the holder quite a bit further than a standard endmill of comparable dia.
Great write up, points i have not thought of
 
As those that have used these have said they are a specialised tool. I have used them in toolmaking to rough out cavities and in on stamping dies. There are multi fluters with a long flute length for side milling. In my experience unless they are in a sidekick they will pull out if used aggressively. As Marcus said it's cheating using a pocket of that shape. Show it doing full 3d with tight corners and steep walls at high speed and you will grab my attention. These cutters really shine in less rigid machines with the way they load up through the spindle. My one big question would be why are they sending Marcus info about tech that I have used for 20 plus years, it's not like it's new.
 
My one big question would be why are they sending Marcus info about tech that I have used for 20 plus years, it's not like it's new.
Whether he loves them or hates them, he went to a web forum, posted about it, got us all to look at it and now we're discussing it. Marketing people lay awake at night, dreaming of that kind of engagement.

I think Marcus is their mole.
 
Bad Marcus, bad bad Marcus. Logical questions and thoughts against the advertiser will not be tolerated. Get back in line.
 
Whether he loves them or hates them, he went to a web forum, posted about it, got us all to look at it and now we're discussing it. Marketing people lay awake at night, dreaming of that kind of engagement.

I think Marcus is their mole.
As long as he is not their troll I'm happy. I suppose the marketing guy will get a bonus because no one will bother to correlate sales figures with social media posts.
 
As long as we're all here talking about odd endmills, when I first saw the video, I wondered if it had a reduced shank so it could do detail work wayyy down in a pocket and still have the rigidity of the solid shank.

No on this one but, does anyone have a source of necked endmills (I current need a 1/4")? I need to cut a D shape pocket at the bottom of a 0.612" diameter bore. I don't have a grinder to do my own.
 
Hi Donkey Hotey.
Mari Tool sells them, and the best thing about Frank's offering is that the reduced shank is the full length of the shank, so a 1/4' diameter cutter will have a 6 mm shank.
That way you can hang it out whatever length you want to and are not restricted in the way you are if the cutter is necked only to a specific length.
I like them...they are nice cutters and cut well, and Frank appears to be a great guy judging from the posts he writes on here.

There are others who sell these now too, but I believe Frank was the first on the block, and since I like to buy from the smaller guy when I can, he gets the sale whenever his offerings meet my needs.

Here's a link:

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Thanks for the kind words implex!

I enjoy carrying solutions. Everyone stocks a 1/2" carbide 4 flute end mill. I like to be known as the vendor that stocks those odd ball solutions that will then engrave our name in your memory for future !!

Our reduced shank endmills have been a nice line for us. It was a huge solution for me back in my job shop years. I am even having custom hydraulic sleeves to work with our reduced shank endmills so you have even more options.

Same goes with our multi reach solid carbide boring, grooving, and threading bars and ER-Hex collets, and ER extended nose collets. Oddball stuff but sometimes a life saver.
 
Just realized this is a Harvey post.
Harvey has great products and they have been around a long time. They also carry some really unique tools and should be book marked in every machinists web browser!
 
Good morning gregormarwick:
I just read your post #15 more carefully, and I have to ask:
You wrote:
"If you were to do this bottom up with adaptive toolpaths, you'd be either be left with big steps that would need a secondary roughing op, or you'd be taking very small steps in Z which would completely negate the MRR argument."

Why do you believe that?
If I do an fully enclosed pocket with a 45 degree wall and I choose a radial WOC of 0.010" for arguments sake, I can do a step up of 0.010" as well and suffer no real time penalty compared to doing a step up of 0.100"
I simply step up after every single pass instead of every 10 passes, and the time burden of doing the step up is trivial...fractions of a second to reposition in Z.

Also, an "Adaptive Roughing Strategy" (as HSMWorks calls it) will cut an enclosed pocket in a continuous cutting motion until it reaches a point where it has to break up the cut in order to keep the chipload constant...so in this case it will begin to air cut on the return move as soon as it's milled out to the periphery of the pocket at its narrowest point.
I can set the return (air cutting) feedrate to whatever I want, and it's commonly set to the fastest the machine control can handle, so I don't lose a lot there either.

That's almost as efficient for that shape of pocket as what I saw with the high feed endmill, and I believe it's kinder to the cutter and kinder to the machine too, as well as putting less stresss into the workpiece.
I say this because I can drop a cutter into a block almost all the way through, leaving a floor thickness of maybe 0.100" on a 3x3 pocket and have that floor come out very flat with adaptive rough...more so than I can with an old fashioned "drop down in increments" strategy.

On some of the freaky sex toys I cut in titanium or 316 stainless, I routinely rough to within 0.005" with a 0.005" step up and the wall thickness of my part is typically 1/16" or less.
I've NEVER failed to clean it up so I have confidence nothing is moving during the roughing.

It sure SOUNDS a lot kinder. and if the WOC and feedrate is calculated well, it's very fast as many of you already know well.

So yeah...I remain unimpressed with those high feed cutters, and that video did nothing to make me change my mind.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Good morning gregormarwick:
I just read your post #15 more carefully, and I have to ask:
You wrote:
"If you were to do this bottom up with adaptive toolpaths, you'd be either be left with big steps that would need a secondary roughing op, or you'd be taking very small steps in Z which would completely negate the MRR argument."

Why do you believe that?
If I do an fully enclosed pocket with a 45 degree wall and I choose a radial WOC of 0.010" for arguments sake, I can do a step up of 0.010" as well and suffer no real time penalty compared to doing a step up of 0.100"
I simply step up after every single pass instead of every 10 passes, and the time burden of doing the step up is trivial...fractions of a second to reposition in Z.

I'll be honest Marcus, you kind of lost me with this! I re-read that several times and I don't follow you. Maybe a screenshot of a toolpath would help me understand what you mean? When I do step up roughing with an endmill I am usually using adaptive stepovers and the full length of the endmill. This provides massive MRR, but leaves stair steps on non-vertical walls.

Maybe worth mentioning that we are at different ends of the spectrum here - my frame of reference is high feed tools in the 60-120mm range on 50 taper machines. The smallest high feed tool I own is a 16mm modular solid carbide from Horn.
 
Hi again Gregor:
In its most basic form, your step up can be the same as your radial stepover if your pocket walls are 45 degrees and your pocket is circular...you will lose no time with this very small step up.
If my stepover is 0.010" and my step up is also 0.010", I will do one circuit around the wall cutting a swath 0.010" thick, before I invoke my next step up, and then I do another single circuit around the wall.
With a rectangular pocket, obviously you have to clear the corners too, but the principle holds that for a 45 degree wall pocket, when you cannot take more than 0.010" bites, you will be just efficient in the roughing with the small step up, because all the extra cuts you do in the roughing to pick out the corners you don't have to do in a semi finishing step, and your part is nearer to net shape with the very efficient roughing strategy.
At least that's my belief and I've done informal time comparisons with co-workers that makes me say so.

If the walls are vertical or near vertical, it obviously matters less and less what the step up is...with vertical walls there need be no step up at all.

With the high feed strategy, you can get close to the same near net shape if you restrict the axial DOC, but when you do, don't you have to take just as many passes?
So to my mind, a 1/2" cutter with a 0.010" stepdown takes just as many passes as a cutter buried 1/2" into a block taking a radial WOC of 0.010".
Each pass still takes a swathe 0.500" x 0.010", but with Adaptive you're not beating the shit out of the corners of the cutter...the load is distributed over the whole flute length.
With a high feed cutter you can only improve your MRR with a bigger cutter or a bigger DOC or a faster feedrate...with a conventional cutter using Adaptive you make the gain with a bigger radial WOC or a faster feedrate or a deeper DOC, and you don't have the restrictions a high feed cutter imposes (according to Carbide Bob), so if you want to cut right up to a vertical wall you can.

So assuming you want to end up with the same roughed shape, I fail to see what the high feed cutter really gains you and with Adaptive, I believe that overall a small step up for a strongly tapered wall gains you lots and doesn't cost you anything in time compared to a big step up and a necessary semifinishing step.
Mind you, if the shape you're cutting is very shallow, the high feed cutter lets you bomb along taking the same amount of material away with every pass, whereas with adaptive you waste more and more time cutting less and less material per pass unless you optimize by jacking up your WOC or your feedrate as you get closer and closer to the top surface of your pocket
So theoretically, your bottom passes are trochoidal (deep DOC but small stepover) but your top passes are more like high feed passes (shallow DOC but big stepover) if you hope to fully optimize your MRR, assuming a pocket with a substantially tapered wall.

If it's a vertical walled pocket of any depth and if Carbide Bob's description is correct, then high feed is useless in that application because you have to leave so much stock near the bottom to avoid trashing the cutter.

On a last note...yeah I'm probably not the guy to talk about hogging big parts...a 1/8" diameter cutter is a monster for me. :D

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
 
Last edited:
Mari Tool sells them, and the best thing about Frank's offering is that the reduced shank is the full length of the shank, so a 1/4' diameter cutter will have a 6 mm shank.
Our reduced shank endmills have been a nice line for us.
Thanks guys. I have a bunch of Mari stuff and so do my friends when I'm done telling them about it. I knew I had seen them somewhere but, couldn't remember where.
 
Well it looks like that video is advertising something that I have been using the last 25 years, starting with the LMT Fette I used. That tool is doing exactly what it is supposed to be doing, long reach high feed roughing, using chip thinning on the BOTTOM of the tool.
Using that strategy is common place in hardmilling mold work, they run for hours unattended on hard mold steels. Your suggestion does not work well for long reach hard material applications, however would be faster on softer pre-heat treat conditions. I have tried both and will always use the video strategy in every circumstance, only not with Harvey tools. I don't cut the funky materials you cut however.
 
Last edited:








 
Back
Top