How would you go about cutting this nozzle cavity?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    3

    Default How would you go about cutting this nozzle cavity?

    I'm looking for suggestions on the best way to cut this nozzle cavity. There are 3 steps, all flat bottom. diameters ranging from .098 to .272". All diameters have a +.000, -.001 tolerance. All 3 diameters have a nozzle that gets pressed into them. The press fit needs to retain the nozzle, and seal. What makes this the most difficult of all is sometimes I have to have my tooling sticking out 4-5 inches. Currently the way I am cutting these is with a helix cycle followed by an interpolated circle to finish. I'm leaning towards getting a custom form tool made to cut this, but the depths and diameters change quite often from part to part.
    I'm having a huge problem with tool deflection cutting them the way I am. Management just tells me to "ream" them with a reamer ground flat. However I don't agree with doing that. Does anyone have any suggestions as to how we can do this better? There has to be a better way!
    We machine these cavity's into lots of different materials... Acetal, aluminum, 1018, 4140, a2. So you can imagine my issues in the harder materials with lots of tool stickout.

    1.jpg
    2.jpg

    Thanks for any help!
    Josh

  2. #2
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    46
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    1

    Default

    Hate to tell you but you pictures really don't tell us anything useful for dimensions. Also from the description, for your method I assume you're doing this on a mill? and not a lathe?

  3. #3
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    505
    Post Thanks / Like
    Likes (Given)
    339
    Likes (Received)
    188

    Default

    yikes...even on the .272" hole you're talking like 14X...is there any way to get shorter gage length?

  4. #4
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    3

    Default

    Sorry, Yes I am cutting on a 3 axis mill. When I have the long stick outs I hold the end mills in an accu-hold. So its not like its a 1/16" end mill sticking out that far. But still far from ideal
    Of the cavity pictured, the 3 diameters are .249,.188,.098. Each "step" is about .1" deep.

  5. #5
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    3

    Default

    I typically cut most diameters with a .093" endmill, but I do use a .0625" EM on the .098 diameter.

  6. #6
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    4,433
    Post Thanks / Like
    Likes (Given)
    106
    Likes (Received)
    622

    Default

    What is preventing you from using long-gauge-length collet chucks or shrink fit holders with short tools? I can't tell from the drawing. Anything stopping you from single-point boring the holes? Obviously a .098" boring tool 5" long is not going to fly, but what is causing the long reach? Can you get a boring head up close so the boring bar itself can be short but the shank of the boring head can be a little long? How many of these parts do you make at a shot?

  7. #7
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    3

    Default

    A boring head is an option I guess, We do LOTS of these in lots of different configurations. usually only a few at a time, but lots throughout the week. The reason for the long stick outs is we put these cavitys on angles typically, and I have to clear the body of the part while it is set up on the angle. Attached is a better pic showing why I have to have stick out. There is very little clearance to the body of the part. I am using a 3/8" accuhold and I am just about rubbing. The tip of my pen represents the pocket I'm cutting. This particular part is 3.7 inches tall, I think I ended up needing the accuhold to stick out like 2.4 inches to clear.

    3.jpg

  8. #8
    Join Date
    Jan 2009
    Location
    "Stuck in Lodi", Ca
    Posts
    3,075
    Post Thanks / Like
    Likes (Given)
    1812
    Likes (Received)
    1586

    Default

    EDM...That's all I got...

  9. #9
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    1,971
    Post Thanks / Like
    Likes (Given)
    557
    Likes (Received)
    994

    Default

    I'm not sure I understand the question, unless the word 'cheap' should be in the Thread title. There are solutions, without question. Here is a link to the Big Kaiser small boring heads (PDF) that will get you exactly what you want.

    http://us.bigkaiser.com/pdfs/KAISER%...874946#page=53

  10. #10
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    2,555
    Post Thanks / Like
    Likes (Given)
    523
    Likes (Received)
    1249

    Default

    Your parts or customer's parts?

    If your parts, kick the designer in the nuts and tell him to make that in 2 pieces.

  11. Likes Nerdlinger, yardbird, awander liked this post
  12. #11
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,103
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1387

    Default

    Hi Josh:
    If you're basically doing OK by helical and circle milling these I'd be inclined to improve that method to eliminate deflection and chatter.
    The best way I can think of to achieve that is to have custom carbide end mills ground up with the biggest longest shanks you can get away with.
    Predrill all you can with a custom HSS step drill so it's a one-shot deal to knock out the worst of the meat, then kiss the sidewalls as you're doing but with your nice stiff cutters that have no setscrews or collets or shrink fits or anything to compromise their rigidity.

    Alfred Lyon at AB Tools will happily grind you up cutters like this and they're not that expensive compared to farting around with tiny boring bars and whatnot.
    If your smallest diameter is 0.098", I'd go with a 2 mm diameter 4 flute cutter with a 0.125" flute depth, necked back to allow you to mill all three steps with the same tool and a 3/8" shank if you can still clear the corners of the part with your biggest orbit using that size shank.
    If you can squeeze in an even bigger shank; do that!

    Plan to kiss out 0.005" or so after your step drilling procedure.
    Using that approach you should do pretty good and if your boss squawks about the price of the cutters tell him to piss off!

    It's a bit of a shitty job so you deserve to have decent tools to make it easier for you.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    www.vancouverwireedm.com

  13. Likes Nerdlinger, scadvice liked this post
  14. #12
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    127
    Post Thanks / Like
    Likes (Given)
    12
    Likes (Received)
    47

    Default

    The boss wants you to try reamers, then try reamers. They should work fine in the softer materials up to 1018 and maybe even the 4140. A2 may be a different story. Then when it doesn't work, the boss can't complain.

  15. Likes digger doug, Nerdlinger liked this post
  16. #13
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    93
    Post Thanks / Like
    Likes (Given)
    108
    Likes (Received)
    49

    Default

    Can you use a custom form tool? Like a port cutter? Might want to rough it out first, but might be able to finish all 3 steps in one plunge?

    Something like this:
    porttools-300x300-circle.jpg

  17. Likes B-Mathews liked this post
  18. #14
    Join Date
    Dec 2004
    Location
    uk
    Posts
    11,975
    Post Thanks / Like
    Likes (Given)
    3230
    Likes (Received)
    5245

    Default

    If that ports common on multiple bits a port cutter is the way to go, there very low cost per hole, just drill a pilot and then plunge it on in here all done in one hit.

  19. #15
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,474
    Post Thanks / Like
    Likes (Given)
    612
    Likes (Received)
    525

    Default

    No matter what sort of tool you use, you still have to reach that far, I see custom cutting tool with multiple diameters on it, or like mentioned before, edm it.

  20. #16
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,103
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1387

    Default

    Hi All:
    The OP posted this in his first post:
    " but the depths and diameters change quite often from part to part."
    So I predict a lot of lightly used form cutters in the toolbox gathering expensive dust if the form changes frequently.

    Milling or boring is awfully attractive in that scenario; I wouldn't personally sinker EDM it for two reasons.

    First; the OP mentioned this:
    "
    lots of different materials... Acetal..."

    Second, EDM is slow and expensive and means farming the work out or getting a machine just to do this operation.
    I have a hard time seeing this fly past management but I may be wrong.
    The OP could certainly suggest it and see what they say.


    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    www.vancouverwireedm.com



  21. #17
    Join Date
    May 2005
    Location
    CA
    Posts
    873
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    138

    Default

    Vancbiker hit the nail on the head.


    PM

  22. #18
    Join Date
    Feb 2013
    Location
    Northern Mn
    Posts
    351
    Post Thanks / Like
    Likes (Given)
    76
    Likes (Received)
    385

    Default

    I have to do a lot of similar holes with extended reach issues (due to fixturing on the multi-axis machines). We have ad some success with custom ground tools. Often times, it is built from the largest carbide blank that we can fit down there. Once the tool is right, it repeats with boring regularity, but the tools are reasonably expensive, and obviously not flexible for alternate hole sizes.

    Most of the time, I just helically bore them. I have a collection of long ER16 holders. Then I use what I call "Old School" endmills. They are 3/8" shank, with a .0625" cutter. They are stupid cheap, especially in HSS... double ended. I keep these segregated from the general population and only use them on this type of hole. Once set with cutter comp, I get thousands of holes without issue (in aluminum).

  23. #19
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    3

    Default

    Thanks everyone for the responses! Lots of good ideas.

    I think I try getting a custom endmill made, as well as getting a few form tools made up. Management has to realize this stuff isn't always cheap.

    Has anyone ever used a bottom cutting reamer? I wasn't aware that they made them, but I found some on line. Yankee makes some custom. I may give those a try as well.

    As for if these are customer parts or our parts... they are our parts... We have all gone at it with the engineers dozens of times but it doesn't seem to do too much good.

  24. #20
    Join Date
    Jan 2014
    Location
    Vancouver, WA. USA
    Posts
    2,555
    Post Thanks / Like
    Likes (Given)
    523
    Likes (Received)
    1249

    Default

    Quote Originally Posted by Js17hilton View Post
    ..... they are our parts... We have all gone at it with the engineers dozens of times but it doesn't seem to do too much good.
    Invite them to participate in the struggle to make good parts might help.

    Years ago I argued some with an engineer about how to remove a bad bearing from a new gearbox he designed. He said the bearing would last the life of the gears. I told him to humor me and consider then that a bearing may be bad from the supplier or damaged at installation. Would he want a gearbox scrapped (pretty big money) because there was no way to remove and replace a bearing without damaging the gearbox? He then said that would be a supplier problem or an assembly problem, not his. Made a visit to the engineering manager and discussed my concerns. A couple days later there was a revised design....

  25. Likes Js17hilton, Nerdlinger liked this post

Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •