How to manufacture this nozzle?

[s4thishkmr]

Hi guys ,

Need help and suggestion in finding best way to manufacturing this nozzle.

Thanks

 

[BvU]

Helli S4, !

Any further constraints ? Material ?

On first sight I would say: drill a hole and use a conical reamer

 

[s4thishkmr]

If I am right : drill two holes top and bottom then to use conical reamer ??

Material aluminium

 

[AZFIREBALL]

Make a casting with a core for tapered hole then machine.

 

[BvU]

How critical is the exact shape of the exit hole ?
And the skewness of the cone -- can it be a straight one ?

 

[s4thishkmr]

Make a casting with a core for tapered hole then machine.

Yeah thank you ..
but I need very less quantity. So I thought any other possibilities

 

[s4thishkmr]

How critical is the exact shape of the exit hole ?
And the skewness of the cone -- can it be a straight one ?

Entry and exit can be straight hole . But cannot be straight throughout.

exit hole should deviate from the center.

Application: when the nozzle rotates , the flow through the exit will form a circle.

Thanks

 

[BvU]

Not what I meant: a straight cone has an elliptical exit hole. Since your cone is only slightly skew, the deviation from circular will be small and might be acceptable.
Entrance hole same story.
The axis of the cone is obviously at an angle wrt both vertical and horizontal in the drawing. (Does G really need to be below center ?)

 

[jrmichler]

Two thoughts:
1) Drill a large hole most of the way through, then drill a small hole from the other end at an angle.
2) Make the nozzle by 3D printing. Then you could make a curved hole if you wanted.

Is it important that the hole be tapered?

 

[AZFIREBALL]

Is G required?

 

[s4thishkmr]

Is G required?

The hole entry should be with 21mm and it should end with 4mm, which deviates 16mm from center.

There is no other constraints.

Thank you

 

[s4thishkmr]

Not what I meant: a straight cone has an elliptical exit hole. Since your cone is only slightly skew, the deviation from circular will be small and might be acceptable.
Entrance hole same story.
The axis of the cone is obviously at an angle wrt both vertical and horizontal in the drawing. (Does G really need to be below center ?)

The hole entry should be with 21mm and it should end with 4mm, which deviates 16mm from center.

There is no other constraints.

 

[s4thishkmr]

Two thoughts:
1) Drill a large hole most of the way through, then drill a small hole from the other end at an angle.
2) Make the nozzle by 3D printing. Then you could make a curved hole if you wanted.

Is it important that the hole be tapered?

Yeah it has to be tapered. Means there can't be any step in between

 

[s4thishkmr]

If I am right : drill two holes top and bottom then to use conical reamer ??

Material aluminium

Sounds feasible. Thank you
I will have try that

 

[Ranger Mike]

I do not think the thread will permit 3D build in a 3D metal printer. Otherwise it could easily be printed in aluminum, steel titanium or Inconel.
you need CAD for it as well. You could print i n aluminum with thread area over size and final machine threads

 

[AZFIREBALL]

Can you make it this way?

 

[s4thishkmr]

Can you make it this way?
View attachment 240429

No it will not work .

Thanks

 

[s4thishkmr]

I do not think the thread will permit 3D build in a 3D metal printer. Otherwise it could easily be printed in aluminum, steel titanium or Inconel.
you need CAD for it as well. You could print i n aluminum with thread area over size and final machine threads

Thank you..
I will try for this as well

 

[AZFIREBALL]

No it will not work .

May I be allowed to know why?

 

[s4thishkmr]

May I be allowed to know why?

I did a similar design and the flow did not come well .

 

[Ranger Mike]

what type 3 D metal printer did you use. what material? how long ago? The part , both in fact are simple to print. the thread area is my only doubt.
2 years ago the part may not have been printed with good result but todays technology has changed.
btw, i sell 3D metal printers and coordinate measuring machines, CT scanners to check porosity of the part.

 

[Claudia Zhou]

Hi s4thishkmr,

Would you like to consider 3D printing plus CNC machining for manufacturing this nozzle?

 

[jrmichler]

3D printing makes excellent nozzles. For an example of a nozzle with curved and tapered holes, see US patent 10,011,450. The nozzles were used directly from the 3D printer without any additional machining.

 

[s4thishkmr]

Thank you guys,

i am going try with metal 3d printing.

 

[Greg London]

You could manufacture that part if you have access to manual machining
equipment including
(1) lathe with a boring bar that fits through a 4mm hole
(2) vertical milling machine, with an endmill with 70mm long cutting surface.
(3) tilting rotary table, preferably with a 3 jaw chuck.

start with a piece of round stock, ~80mm long and ~60mm diameter.
Put it on a manual lathe.
Drill a 4mm hole through the center of the work.
Set the cross slide to 22 degrees(*) off from straight into the work.
Install a boring bar that can fit into a 4mm hole.
Using the boring bar and cross slide, make a tapered internal cut.
repeat until the cutting tool gets to the opening on the other end
(opening on other end should be 4mm still.)

The angles should work out that if you measure from teh 4mm opening
and measure in 48mm, the hole should be 21 mm in diameter.
The opening at the end opposite the 4mm opening will be larger than 21mm
but that's because you'll need more material on that end for the next step.

mount part to center of rotary table that can tilt.
Rotary table with a 3 jaw chuck would be best.
This will allow you to grip onto base of part.
You want the 4mm opening facing up and away from the rotary table.
you want the big end of the opening facing down and clamped by the chuck.
The length of the part clamped onto by the 3 jaw chuck is the extra
material we needed on teh part from the lathe.
This is why the part starts out longer than needed.

Mount rotary table to table of vertical milling machine,
with the spindle coming down into the face of the rotary table.
set angle rotary table to 22 degrees.(*)

Put an endmill with side cutting faces in quill.
Want an endmill that has a side-cutting length of at least 70mm.
lower top of endmill so that cutting edge covers as much of part as possible.
but make sure endmill is ABOVE 3 jaw chuck of rotary table.

lock quill feed so endmill doesn't pull quill down as it cuts.
One side of part will stick out more from center than the rest.
turn rotary table to put this side closest to endmill.
turn on mill
move mill table left/right which ever direction gets part closer to endmill cutter.
once part contacts endmill, continue for whatever your cutting depth is.
now rotate table so part meets endmill cutting surface in a conventional cut.
rotate table one revolution.

turn crank on milling maching table moving table left/right,
move table so that part is one cutting depth closer to endmill,
turn the rotary table one revolution.
move part closer to endmill, turn rotary table one revolution.
repeat until end of endmill is in contact with part.
This means that

The rotary table will eventually re-face the part so that the axis of the
internal channel is out of round to the axis of the outside surface.

Remove part from rotary table.

Base of part that was in 3 jaw chuck will be off kiltered.
put part back in lathe, but have the off-kiltered end sticking out.
use indicator to verify part nearest chuck is centered as much as possible.
lathe off-kiltered portion down to match the rest of part.
this may result in a slight ridge where this new lathed surface meets
the surface cut by the milling machine.

Use a cut off tool to get part to desired length.
you should now have an opening that is 4mm on one end and 21mm on other.

Lathe should then be able to cut the step on the part so that
surface for threads is at correct diameter.
The threads you've spec'ed are impossible to cut on a lathe.
Not sure you could do it with a die either.

Generally, you need a chunk of the part past the threads that is undercut.
As the lathe is cutting the threads, teh undercut portion gives the
operator time to stop the lathe. If you use a die, the start of the die
makes a shallower cut than the end of the die. So, if you want fully cut threads
for 8.5 mm, you will need to lathe down the part to 8.5mm plus the thickness of the die.
If you lathe the threads manually, you'll probably want 8.5mm at correct diameter
and then 10mm that is undercut.

So, lathe out the diameter for threads.
If lathing the threads, add 10mm of undercut.
If using a die, lathe out 8.5+die thickness at the diameter for thread.

Then do the threads.

Put a 45 degree chamber on corners of part,
flip part around in lathe and chamfer other side too.

Viola. you've got your part.

If you have access to machining equipment,
you could probably do this in a day.

(*) Footnote: I guestimated the angle.
you'd need to do some trig to figure out the exact angles needed.

 

[Greg London]

Whoops. Not quite right. Not a tilting rotary table. You need a rotary table with a 22 degree spacer under the part. The axis of the table should be straight up. The part should be on top of a spacer to tilt it at correct angle.

Everything else should work.

 

[Mech_Engineer]

You could wire EDM (Electro-Discharge Machining) this feature. Wire EDM uses a very thin wire that can cut through conductive materials and should be able to do a tilted/tapered cone like this.

More reading: http://www.edmmachining.com/wire_edm.htm