Need help from all the machinist on this forum - Page 1
Forum section: electronics / general

author: DavidDLC
author_rank: Frequent Contributor
timestamp: April 18, 2015, 08:10:44 pm
content: Hi guys,I'm a machinist apprentice.I need to buy an end mill that has a relative long cut section like 2 inches, diameter can be 1/4, 5/16, 3/8How should I look for it ?I already googled it: Long cut end mill and similar but nothing found.I have this link, but not sure if it is what I'm looking for:http://www.amazon.com/Flute-Single-End-Mills-Length/dp/B006Q4YVN6/ref=sr_1_30?ie=UTF8&qid=1429239079&sr=8-30&keywords=5%2F16+x+2+end+millPlease comment, I don't want something super expensive.David.

author: PeterFW
author_rank: Frequent Contributor
timestamp: April 18, 2015, 08:28:05 pm
content: Quote from: DavidDLC on April 18, 2015, 08:10:44 pmTher is only a little bit i know about milling but you should include:Type of material to be milledType of surface finish after millingType of shape to be milledThere are so many different types ot bits...Greetings,Peter

author: DavidDLC
author_rank: Frequent Contributor
timestamp: April 18, 2015, 08:31:39 pm
content: Type of material to be milled: AluminumType of surface finish after milling: It does not matter muchType of shape to be milled: Flat or straight.It is a bar, so I cannot use like a flycutter, it has to be a end mill.David.

author: Andy Watson
author_rank: Super Contributor
timestamp: April 18, 2015, 08:41:09 pm
content: Try searching for "Extra long slot drill". Although, 2" extension at 1/4 diameter is pushing it!"Long series slot drill" might also work.

author: PeterFW
author_rank: Frequent Contributor
timestamp: April 18, 2015, 08:54:18 pm
content: Quote from: DavidDLC on April 18, 2015, 08:31:39 pmThere are sooooo many different types of aluminum....Search for "Extra long end mill", at that diameter and lengh i would be very, very carefull.Carbine is damn brittle, here you got a 2 flute square end (Googled it, no idea about the shop)But this is a bit out of my comfort zone, my bits are a tad smaller.Last one i ordered was a 0.6mm single flutehttp://www.the-carbide-end-mill-store.com/20m5/square-end-mills/xx-long-length/2-flutes/uncoated.htmlYou might want to look into HSS with carbide tips, if you only need to route a bit with it you might get away with a "cheap one" for wood.

author: ManCave
author_rank: Regular Contributor
timestamp: April 18, 2015, 09:18:08 pm
content: Have a look at the MSC (UK) website. I appreciate that you are in the US and probably won't be able to buy from them, but their catalogue (accessible online) has explanations on mill bits selection.Go to theirWebsiteand have a look into the virtual catalogue. On page 293 they have the milling section and if you go page by page from there you should get enough info to be able to choose.Hope this helps!

author: Lightages
author_rank: Unknown
timestamp: April 18, 2015, 09:40:03 pm
content: I have used this company many times. I found them to have good service and almost everything that I have needed. Specifically for you:http://www.use-enco.com/CGI/INSRIT?PARTPG=INSRAR2&PMAKA=337-5925&PMPXNO=28077301

author: DavidDLC
author_rank: Frequent Contributor
timestamp: April 18, 2015, 10:13:08 pm
content: Quote from: Lightages on April 18, 2015, 09:40:03 pmI like the price !Gracias Lightages.

author: rx8pilot
author_rank: Super Contributor
timestamp: April 21, 2015, 05:57:25 pm
content: Quote from: DavidDLC on April 18, 2015, 08:10:44 pmA long 'Depth of Cut' DOC is not a practical technique for machining. You will find trouble if the depth goes beyond 2x the diameter of the tool. So, for a 1/4" tool, a 1/2" wall is reasonable. The problem is that the tool being engaged with so much material at one time is beyond the strength of the tool and it will chatter - essentially bouncing off the surface you are trying to cut. When you get into a corner, it becomes much worse as the tool engages more material. The vibrations will damage the tool while leaving a very poor surface finish. When I was a younger machinist I purchased a few long flute tools and learned very quickly that they are very hard to use. If you are very patient, you may be able to find a combination of rpm-feed rate-axial depth of cut that can work. It will generally be a heavy chip load scenario with low rpm compared to feed rate. Keeping the tool loaded will reduce chatter.I take a different approach and use reduced shank tools. They have a flute length that is about the same as the diameter of the tool and the shank is reduced to about .025" less than the cutting flutes. This arrangement allows you to step down the wall without over engaging the tool or having the shank rubbing the wall as you would with a normal tool. I doubt you will find them at Enco since they are generally a high-end solution.http://www.harveytool.com/prod/Browse-Our-Products/Signature-Series--Miniature-End-Mills-/Corner-Radius-Miniature-End-Mills_182/End-Mills---Corner-Radius-Reduced-Shank-End-Mills_119.aspxThe corner radius on the end is important to blend each pass of the tool. A sharp corner will leave steps on the wall.

author: skipjackrc4
author_rank: Regular Contributor
timestamp: April 21, 2015, 07:30:07 pm
content: I needed a similar depth of cut in ABS plastic, so I bought a carbide router bit for wood working. It works beautifully, and cuts Al quite well also. It's not as rigid as an equivalently sized end mill, but in soft materials with low feed rates, it works just fine. No way would I try that on steel though.

author: G7PSK
author_rank: Super Contributor
timestamp: April 21, 2015, 08:20:21 pm
content: Must it be an end mill,can you not use a slitter or a ripper.

author: robrenz
author_rank: Super Contributor
timestamp: April 21, 2015, 08:23:32 pm
content: If you really need 1/4 - 3/8 dia x 2" length of cut these things will help.1. Carbide for 3X higher modulus of elasticity (deflects less)2. Hi flute count like 5 or higher. As the flute count goes up the flute depth goes down giving a larger diameter core (deflects less)3. Higher helix than normal like 37 or 45 degree. This makes the cutting forces shift toward axial from radial. (tends to lower chatter tendencies)4. Minimize arc of contact. Don't try to do make a 3/16 radius in a 90 degree internal corner with a 3/8 end mill. Use a smaller end mill and cnc to interpolate the radius and control radial depth of cut to minimize arc of contact.5. Use rougher style with all of the above.6. Use variable helix cutters which tend to dampen harmonics.7. Find the optimum speed for the situation. Google "stability lobe diagrams for machine tools"I do 8X lengths of cut in ductile iron and aluminum on a routine basis but it takes proper techniques like listed above.

author: PeterFW
author_rank: Frequent Contributor
timestamp: April 21, 2015, 08:26:30 pm
content: Quote from: robrenz on April 21, 2015, 08:23:32 pmBut he said that he does not want something super expensive and a bit with the attributes listed above is pretty pricey

author: robrenz
author_rank: Super Contributor
timestamp: April 21, 2015, 08:31:31 pm
content: He mentioned he is an apprentice, I think him gaining an understanding of all the things I mentioned will be very useful to him. Some times if you really have to do something you have to pay for the tool that will do the job.

author: PeterFW
author_rank: Frequent Contributor
timestamp: April 21, 2015, 08:43:10 pm
content: Quote from: robrenz on April 21, 2015, 08:31:31 pmMhm... indeed, you are rightQuoteAnd sometimes you need to be just inventive enough to mis-use another tool that will do the job juuuuust well enough.Besides my decent carbide drills are a few of the cheapest, worst and most horrible china drills that could be made out of hardent lead.If i just have to drill six 50mm hole in some particle board that i can flip over and drill on both sides i will buy a 5 Euro china drill instead of a 40 Euro one anny day of the week.But if i would have to drill 50 of those holes, then i will buy the 50 euro bit

author: rx8pilot
author_rank: Super Contributor
timestamp: April 21, 2015, 09:16:54 pm
content: Quote from: PeterFW on April 21, 2015, 08:26:30 pmFor a cheaper solution - change the design. Deep holes and tight corners are expensive in the machining world. I have been machining for a long time, but 99.9% of it is my own designs so I tend to avoid situations that are difficult when I can. Where a feature needs to be a certain way - just add money and brains to solve it.I have been so frustrated with just-good-enough tools over the years that I just don't buy them anymore. My first milling machine was a cheap Chinese made random brand that I was hoping to learn the basics. I ended up learning how to fix and work around a terrible machine. I had random crap HSS end mills that only taught me the value of the good ones.A note on carbide.....it is rigid as robrenz points out. That also means it is brittle and cracks and shatters far more easily than HSS tools. When operated properly, carbide lasts a very long time in Al and similar materials. One little mistake will snap it half.

author: DavidDLC
author_rank: Frequent Contributor
timestamp: April 25, 2015, 04:19:00 am
content: Definitely I'm learning from here. And yes I'm an apprentice with a small toy mill machine.David.

author: Paul Moir
author_rank: Frequent Contributor
timestamp: April 25, 2015, 04:57:30 am
content: If it's not much of a milling machine, avoid solid carbide. The slop in the machine will cause you to chip the cutter in no time. Unfortunately, HSS tools tend to be cheap junk or somewhat low tech these days.rx8pilot says to change the design, and I'm with him on that. I sort of bridge the gap: sometimes hammering something out on a sloppy cheap manual machine or sometimes drawing for CNC or manual. When I first did drawings, the manual experience I had helped but I would still put my contact info right on the drawing and meet with the machinist to look over my drawings to find trouble spots. I would have appreciated a call that said "this deep thin slot is gonna cost ya!"I've done 1" deep with a 1/4" endmill like the one Lightages points you towards in aluminium (I'm talkin 6061-T6 which is dead easy) without much trouble. It was slow since tool deflection is a real serious problem. 2" makes me shudder, even with a 3/8". If you can mill from both sides (like going through) I would do that if at all possible. Chip evacuation from 2" down itself going to be some work.

author: DavidDLC
author_rank: Frequent Contributor
timestamp: April 25, 2015, 05:10:54 am
content: Quote from: rx8pilot on April 21, 2015, 05:57:25 pmI told you I'm learning, I didn't know these are available.

author: rx8pilot
author_rank: Super Contributor
timestamp: April 25, 2015, 06:15:11 am
content: I hope the notes are helpful. The learning curve in a CNC shop is rather steep. Every once in a while you find a tip or two from someone that struggled with the same problem many years before.

author: robrenz
author_rank: Super Contributor
timestamp: April 25, 2015, 02:33:08 pm
content: Quote from: DavidDLC on April 25, 2015, 04:19:00 amWhen you said apprentice I assumed you were using full size industrial machines. All my suggestions were based on that. I started machining when I was 12 on a Unimat (see pics below). You can actually learn a lot on a flimsy machine about tool forces and deflections, resonant frequencies etc because you can see them happening. Keep on making chips