Author Topic: How can I machine this?  (Read 13067 times)

Offline smooth90

  • Ewok
  • *
  • Posts: 8
    • View Profile
How can I machine this?
« on: June 29, 2011, 22:57:39 pm »
I am trying to make a pulse jet engine with an argus type valve. Below is a picture of one of the reed valve retainers. These are the most complicated parts (geometry wise) in the entire engine.

The part will be machined out of 5/8in thick 1.5in wide aluminum bar that will be cut to the proper length prior to machining. Those are the exact external dimensions of this part meaning that the machining should ONLY be done to cut out the holes, channels, and other features there should be no tool pathways around the perimeter of this block.

The only machine I have is a Fireball V90 cnc router with a Bosch colt router on it. I have metal cutting endmills and ball mills for it as well as a spray mist cooling system hooked up to it. This machine is more than capable of machining aluminum with shallow passes.




Now the part is double sided but that is not the problem. My main issue is cutting the angled cuts which are CRITICAL in the functionality of the pulse jet.

I have pointed arrows toward the problem causing cuts in this picture.






This type of part is something that I would be able to machine immediately notice there are no angles. This would be simple to set up in cambam.












DOES ANYONE HAVE ANY IDEAS??? I would really appreciate any input

thanks.









.

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8909
    • View Profile
Re: How can I machine this?
« Reply #1 on: June 30, 2011, 00:41:09 am »
The part will be machined out of 5/8in thick 1.5in wide aluminum bar that will be cut to the proper length prior to machining. Those are the exact external dimensions of this part meaning that the machining should ONLY be done to cut out the holes, channels, and other features there should be no tool pathways around the perimeter of this block.
--------------------
It makes no sense, unless you cannot afford larger stock, to restrain yourself to "machining around" an imprecisely-extruded or rolled piece of mill stock.  Even if it were cut-to-length, its width and height would be suspect.  If it was "machined all over", then why not let your machine do all of it?  It would be much better to machine the entire part profile to precise dimensions.

The "undercuts" in your retainer prongs are impossible in a 2.5D environment.  If you want, instead, a comb-like structure like your 'bad' CAMBAM picture, then it is quite feasible to do.

Shooting the ramp down the comb is confusing to me to draw in CAMBAM alone.  It's easy to draw in any 3D package, and import as a mesh.  Another better CAMBAM user might have an easy way to do it within CAMBAM.

Doing that slope to any degree of finish is just about impossible on a 2.5D setup unless you use almost microscopic step-overs and a ballnose milling cutter to cut the slope.

LLoyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline gpw

  • Wookie
  • ****
  • Posts: 295
    • View Profile
Re: How can I machine this?
« Reply #2 on: June 30, 2011, 00:53:49 am »
You will experience some movement of the part due to internal stresses which can be minimized by rough machining entirely, and then finish machining.

Cut the angle last with the part on an angle plate or tilting table using a square shoulder face mill or a fly cutter if it is critical. That way the angle will be a flat plane.

I cut these from phenolic laminate using an angle plate.

« Last Edit: June 30, 2011, 00:58:43 am by gpw »

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8909
    • View Profile
Re: How can I machine this?
« Reply #3 on: June 30, 2011, 01:16:26 am »
Cut the angle last with the part on an angle plate or tilting table using a square shoulder face mill or a fly cutter if it is critical. That way the angle will be a flat plane.
-----------

That's a really great idea I somehow overlooked, but I might make one recommendation:

The "fins" of his comb assembly are quite thin, and won't take kindly to machining their tops to cut the slope.  They'll spring - ruining surface finish - or they'll bend.

I'd suggest machining the stock block on an angle plate first, before _any_ other MOps, and then clamp it down square to finish off the profile and pockets between the fins.

LLoyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline gpw

  • Wookie
  • ****
  • Posts: 295
    • View Profile
Re: How can I machine this?
« Reply #4 on: June 30, 2011, 01:26:28 am »
That's a good point!

There are products with a very low melting point to encase such delicate parts for machining in such circumstances.

Depending on how critical the flatness is, that may be an option. (or requirement)

Even something as simple as candle wax may work in this case.

Thanks!
« Last Edit: June 30, 2011, 01:29:16 am by gpw »

Offline lloydsp

  • CNC Jedi
  • *****
  • Posts: 8909
    • View Profile
Re: How can I machine this?
« Reply #5 on: June 30, 2011, 01:56:12 am »
There are products with a very low melting point to encase such delicate parts for machining in such circumstances.

Depending on how critical the flatness is, that may be an option. (or requirement)

Even something as simple as candle wax may work in this case.

-------------------------

I use CerroTrue alloy, but one must be careful how much you machine off, as contaminated chips are hard to re-melt without spoiling the batch, and it's VERY expensive  (about $30/lb ten years ago, when I bought my last ingots of it).

LLoyd
"Pyro for Fun and Profit for More Than Fifty Years"

Offline smooth90

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: How can I machine this?
« Reply #6 on: June 30, 2011, 02:33:14 am »
I am not so concerned with the outer dimensions of the valve. Making a "precise" block of stock in my situation is not feasible. If I had a milling machine with the correct tooling (flycutters...end mills) I wouldn't have an issue doing this but all I have is a cnc router with 1/8in bits.  I would go through bits like crazy if I tried doing the work of a flycutter with an 1/8in bit.

A mill (and metal lathe) are on my list of things to get in about 6 years (after college). I'm only 16 right now so its not like I can run out and get these things  :o  I have spent thousands on tools already...cnc router...miller ac/dc tig welder....various metalworking tools....tons of stuff. Now if you can get minimum wage tripled then I would happily buy a mill  ;D

By using extruded stock I can get uniform width and thickness (to an extent) on all of the stock. I will measure everything with a caliper (to .001") before I start and adjust my 3d models to compensate for any difference. I'm not building a space shuttle here the valves don't have to be absolutely perfect but the angles on the valves have to be as good as possible.

I just did a test using wood to see what the steps would look like and it was exactly as I thought the angled portion look like a staircase. I can reduce the step to something ridiculous or I can build an angle jig as was suggested.

I whipped up an angle jig in Inventor that will adjust the angle of the block such that the angle portion is parallel to the cutting surface. This jig will be made from 2in 1/8in thick aluminum bar. I will cnc cut the important parts and then tig weld the pieces together.

BTW the thin baffles on the part are 3/32in thick which is more then enough to hold up to a 1/8in bit spinning at 35,000rpm.

My plan is to take the aluminum block and use cambam to machine the 2 holes into it as well as a mark as to where the angled notch has to be. This will allow me to attach the block to the jig with bolts. Since the angled surface is now parallel to the cutting head I can use cambam just like if I were maching flat notches into an aluminum bar. Once I line it up to the notch that was made and verifying that everything is level and in line I can run the cnc and have it machine the notches into the bar. Once thats done I can flip the bar over and machine the notches on the other side. Once the angled part is finished I can actually use cambam with flat 2d dxfs to finish making the channels and other features. Then hopefully in the end I should have the finished part....repeat 3 more times and I have enough parts to build the valve.


Here are some pictures












« Last Edit: June 30, 2011, 02:35:15 am by smooth90 »

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3345
    • View Profile
Re: How can I machine this?
« Reply #7 on: June 30, 2011, 23:38:43 pm »
Can you post the stl file? I would like to take a look at it. I do believe it is possible to cut as 3d, but not knowing the dimensions it's hard to suggest proper tooling and approach.
My 2¢

Win11, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, 4th Axis, Endurance Laser.

Offline smooth90

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: How can I machine this?
« Reply #8 on: July 01, 2011, 23:56:08 pm »
I have attached the stl file in this post.

Today I received some of my aluminum bar stock and I was fairly impressed with just how close the dimensions were to there width/height. I measured a 1.5in wide bar and the width and height were within .003in of what it was suppose to be. It might not be perfect but its more than good enough to be used in this project at a fraction of the cost. Now I just have to wait to get my 5/8in 1.5in wide bars so that I can machine the valves. I want to make those first because if I can't make those then the project will be....doomed.


Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3345
    • View Profile
Re: How can I machine this?
« Reply #9 on: July 02, 2011, 14:10:18 pm »
After looking on the file and re-reading what you have work with, I'm afraid you won't be happy with the results to put it nicely. First, I would cut mock-up of the part out of hard wood. You will learn much from it... There is a limit what wood router can do... Good luck.
My 2¢

Win11, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, 4th Axis, Endurance Laser.

Offline gpw

  • Wookie
  • ****
  • Posts: 295
    • View Profile
Re: How can I machine this?
« Reply #10 on: July 02, 2011, 14:26:07 pm »
One concern would be quickly loading the flutes of the small cutters with aluminum and snapping them off. 6061 can be quite gummy to machine dry. I doubt coolant is an option on a router.

Offline smooth90

  • Ewok
  • *
  • Posts: 8
    • View Profile
Re: How can I machine this?
« Reply #11 on: July 03, 2011, 03:30:25 am »
The router has ample power to chew through stuff. I've machined 1/16in 5052 with it before and it chews it to bits like butter. I also have a spray coolant system on my router. I don't use the coolant system often but for metal work it really cools things down.

Keep in mind I'm not going to be taking half inch passes with this thing try .05in for the roughing passes and .005in for the finishing passes. It will take some time to finish machining it but I don't see why it won't work.

I had thoughts about possible problems with the jig idea but I've worked them out. The only issue I see with it is getting the piece lined up to the bit as perfectly as possible. I've added numerous things to my jig design to line the part up as best I can.

I know the world "valve" might make the thought precision pop into your head but this type of valve has some play room. When the engine combustion occurs the pressure increase will slam .01in thick spring steel over these baffles/channels.

I've run every step through my head and feel extremely confident that this is going to work very well but it will be time consuming. At least 6 hours of work per piece (mostly setup and machining time). I plan on doing it step by step repeating the same machining operation of all of the pieces at once to save setup time but still its goining to take a while.


I will post back in a couple weeks with pictures step by step showing how I did it.

Offline Bubba

  • CNC Jedi
  • *****
  • Posts: 3345
    • View Profile
Re: How can I machine this?
« Reply #12 on: July 03, 2011, 12:59:48 pm »
It appears the part is symmetrical. Then, why not use little longer stock, drill couple "alignment/tooling holes" and use in jig to assure perfect location on all operations. If I would machine this, I would machine the outside dimensions to finish, drill the .25" holes in location that is called for, use them to align and clamp the work piece. Then machine the angles, the last step would be the cutouts. Once the top side completed spray the part with mold release, mix a batch of plaster(don't laugh) i use it before with great results, it stops the part from chattering and keeps the part in place. You have to machine dry. I know its a old school of doing thing but... it works. As I said many times before... you don't need any coolant on aluminum as long as you are using sharp cutting tool and a proper feed rate. All those suggestions are for milling on the mill, I do own the machines necessary to do this... In any rate, I hope this give you some perspective of different approaches to this. I'm firm believer there are many ways to get the job done, but.. it is up to an individual to chose the way based on his experience, machine, etc..

HAPPY 4Th TO ALL MY FIENDS IN THE US!
My 2¢

Win11, CB(1.0)rc 1(64 bit) Mach3, ESS, G540, 4th Axis, Endurance Laser.

Offline kvom

  • CNC Jedi
  • *****
  • Posts: 1612
    • View Profile
Re: How can I machine this?
« Reply #13 on: July 03, 2011, 15:08:27 pm »
One concern would be quickly loading the flutes of the small cutters with aluminum and snapping them off. 6061 can be quite gummy to machine dry. I doubt coolant is an option on a router.

use of WD40 or kerosene as a lubricant will help here.

Offline lazer

  • Storm Trooper
  • ***
  • Posts: 201
    • View Profile
Re: How can I machine this?
« Reply #14 on: July 03, 2011, 21:50:35 pm »
Hello Smooth90

I speak little in English.  :D
Analysis photos reed1.jpg and reed2.jpg
See attached file Reed_Cage_Ar1.cb

Armando
« Last Edit: July 03, 2011, 21:52:16 pm by lazer »
lazer = leisure -- Sorry my English