Author Topic: camshaft machining  (Read 932 times)

Offline Gadabout

  • Jr. Member
  • **
  • Posts: 19
camshaft machining
« on: August 06, 2019, 05:07:01 PM »
Hi, I am building the Seal 15cc 4 cylinder engine and want to machine the camshaft on my small cnc mill, The machine has a fourth axis (A) and knee and spindle axis's as well as x and y. I have drawn the two cam profiles( inlet and exhaust) in Solidworks(2001) and have featurecam 5 for cam and mach3 , but I can not get my head around how to get the gcode for the machining of the cam profiles, was thinking of the camshaft axis parallel to the x axis and either using the spindle axis or the knee one for z movement, I think I can hand program the rest of the movements to get the cams in the correct orientation. can anyone help me with what I need to do please as I am not too good at this!!
thanks
Mark

Offline djc

  • Jr. Member
  • **
  • Posts: 46
Re: camshaft machining
« Reply #1 on: August 09, 2019, 03:00:25 PM »
The machine has a fourth axis (A) and knee and spindle axis's

When you say knee and spindle axes, do you mean knee and quill or knee and rotary axis?

I assume if you are outside the cam, it is at every point concave (i.e, you can put a straight edge on it and it will touch at one point only).

Can you post a dimensioned drawing of a typical cam profile? Is it made up solely of circular arcs?

Use the centreline of the cam as your datum. Pick an arbitrary point as your zero rotation. Measure the distance from centre of cam to outer edge. Write it down. Rotate one degree. Repeat. You will get a list of 'coordinate pairs' of angle and Z-height above centre.

Set cutter clear of work. Drop down to Z-height, move in X until cutter is clear of work. Move A-axis one increment on your coordinate pair list, move to new Z-height, move in X until clear of work. Repeat. The smaller the A-axis increments, the smoother your cam will be. If you can define it mathematically, so there is a formulaic connection between A and Z, you can use a spreadsheet to do a lot of the coordinate pair calculation for you.

Offline Gadabout

  • Jr. Member
  • **
  • Posts: 19
Re: camshaft machining
« Reply #2 on: August 09, 2019, 06:11:25 PM »
Djc, thanks for the reply. My mill has cnc on the x,y,z(knee) ,A (rotary table) and B (quill) has vertical as well as horizontal spindles. Mach3 is the controller.
The camshaft in question has eight lobes(4 inlet, 4 exhaust) and I would like to write a gcode program to machine the lobes. I have drawn the lobe profiles in Solidworks 2001 and would like to work out how I write the gcode for the lobe paroles as I can write the rest ok. I will post the cam profiles later when I get to the pc they are on.
Thanks
Mark

Offline chipenter

  • Hero Member
  • *****
  • Posts: 851
  • Country: gb
Re: camshaft machining
« Reply #3 on: August 10, 2019, 01:24:46 AM »
Solidcam is made to do just that , export the drawing into cam it will convert to G code .
Jeff

Offline djc

  • Jr. Member
  • **
  • Posts: 46
Re: camshaft machining
« Reply #4 on: August 10, 2019, 02:47:37 AM »
Solidcam is made to do just that, export the drawing into cam it will convert to G code.

He says he has FeatureCAM.

For his setup, he needs something will output G-code to do simultaneous motion in A- and Z- . This is not quite so easy.

To the OP, have a look on this site for a post by Andrew Mawson entitled 'maths help'. It might look at first sight as if his issue was completely different to your own, but the concept is identical. For every point on the 360 degrees of the circle, you need an equation that tells you the distance of the part edge from the centre of that circle.

For A-axis machining, you can cheat a bit and fool the controller into thinking the A-axis is a linear axis. Effectively, you unwrap the profile from around the circle and turn it into a straight line. Then you can command simultaneous motion in Z- and your-now-linear A- .

Have a look at a program called CNC wrapper. There is also a little bit on this technique in the documentation for Dolphin Partsmaster.

Offline djc

  • Jr. Member
  • **
  • Posts: 46
Re: camshaft machining
« Reply #5 on: August 10, 2019, 04:31:16 AM »
OK, I found the seal drawings on the Model Engineer website.

Attached are some rough sketches (inlet only, right hand sketch). First, because Uncle Ed. did not have the benefit of CAD, his dimensions do not quite work. The combination of 11/32" base, 9/16" flank radius, 1/32" fillet and 5/64" lift do not give a smooth curve. In my sketch, I have used the radii as given: with everything properly tangential, it results in 0.004" less lift. If the lift is critical, you will have to alter one or other of the dimensions.

The cam is symmetrical and only composed of circular arcs. For 240 degrees of its circumference, it is a circle (constant radius) so that bit is easy.

To calculate the Z-dimensions as above posts, the left and centre sketches may help. Start with the centre one. For any angle a [from 0 to 20.4 degrees], measured from the start of the flank radius, you use the cosine rule to calculate x, the distance from the centre of the cam. You also need to calculate the angle from the cam centre at which that distance applies (I did not show that as the sketches are too messy as they are).

Similarly (now use the left sketch), you can calculate y, the distance from cam centre when traversing the fillet radius. Cosine rule again, using angle b [from 0 to 39.5 degrees]. Again, calculate angle from cam centre at which that distance applies.

Now, the most important bit: you will not be able to cut the flank and fillets using a flat-bottomed cutter as the edge of it will dig in where you do not want it. You need to use a ball-ended cutter and then it is always tangential to the cam profile.

Offline philf

  • Hero Member
  • *****
  • Posts: 882
  • Country: gb
Re: camshaft machining
« Reply #6 on: August 10, 2019, 01:42:21 PM »
........................

Now, the most important bit: you will not be able to cut the flank and fillets using a flat-bottomed cutter as the edge of it will dig in where you do not want it. You need to use a ball-ended cutter and then it is always tangential to the cam profile.

I'm puzzled - I have only seen a low resolution section through the engine and the cam follower seems to be flat. For the cam to work properly with a flat follower then that would mean that a cutter could be the same diameter and shape as the follower.

Phil Fern
Location: Marple, Cheshire

Offline chipenter

  • Hero Member
  • *****
  • Posts: 851
  • Country: gb
Re: camshaft machining
« Reply #7 on: August 10, 2019, 03:31:19 PM »
Those angles don't add up the 11/64" radius at 30 degrees the other should be 50.4476 by my reckoning , if using the A and Z axis G2 or G3 I would file the 1/32 radius .
Jeff

Offline djc

  • Jr. Member
  • **
  • Posts: 46
Re: camshaft machining
« Reply #8 on: August 11, 2019, 04:21:46 AM »
Those angles don't add up the 11/64" radius at 30 degrees the other should be 50.4476 by my reckoning.

The three angles on the sketches each have a different vertex. The 30 degree relates to the 11/32" diameter; the 20.4 degree relates to the 9/16" radius; the 39.5 relates to the 1/32" radius.

As you traverse the 9/16" arc and the 1/32" arc, you will subtend an angle of 60 degrees measured from the centre of the 11/32" diameter.

Offline djc

  • Jr. Member
  • **
  • Posts: 46
Re: camshaft machining
« Reply #9 on: August 11, 2019, 04:53:20 AM »
I'm puzzled - I have only seen a low resolution section through the engine and the cam follower seems to be flat. For the cam to work properly with a flat follower then that would mean that a cutter could be the same diameter and shape as the follower.

I see what you are saying and in my initial reply, I thought a flat cutter would be OK. It is only when you draw the geometry that you see what is going on.

There is a difference between a follower moving on a cam and a sharp rotatey thing cutting chunks out of a cam blank to produce a defined shape.

Using a flat follower on this cam will result in the fully closed or open position varying depending on the width of the follower. If the follower is of zero width, fully closed will be at the 30 degree position. If the follower is quite wide, the edge of it will start to ride up the 9/16" radius before its centre intersects the 30 degree position. If the edge of it is sharp and not able to ride, it will cut out part of the cam.

There is one of the old Machinery's yellow cover textbooks on the Internet Archive that covers cam design. It is an interesting read. Varying the position and shape of the follower on the same cam can make a big difference to its movement. You have to start with either a cam geometry or a movement profile and then design the rest to suit. Here, we are wanting to reproduce as accurately as we can, what Mr Westbury first drew.

Offline Gadabout

  • Jr. Member
  • **
  • Posts: 19
Re: camshaft machining
« Reply #10 on: August 11, 2019, 05:14:03 PM »
Wow, thanks guys for all the input! Its all much appreciated!!
Djc thanks for the drawings, unfortunately I have no idea what they mean!! maths and I parted ways some 45 years ago when I left school!! Suppose I could go to the cad drawing and just take measurements every couple of degrees for the a and z positions its just that I was thinking there must be a better solution where the gcode would be automatically generated.
thanks
Mark

Offline Gadabout

  • Jr. Member
  • **
  • Posts: 19
Re: camshaft machining
« Reply #11 on: August 11, 2019, 11:01:11 PM »
What about this ? http://gcam.lucasemail.org/  could it be adapted? 
cheers
Mark

Offline djc

  • Jr. Member
  • **
  • Posts: 46
Re: camshaft machining
« Reply #12 on: August 12, 2019, 02:41:15 PM »
What about this ? http://gcam.lucasemail.org/  could it be adapted?

Yes, so long as your spindle axis is parallel to your rotary axis. The challenge with this method, especially for a multi-lobed cam is setting up the tooling. The cutting edge needs to relatively large diameter and approximately the width of the cam lobe. The shank or arbor of the cutting tool needs to be narrow enough to clear the high point of the other cam lobes. As well as the setup in the gcam pictures (where the spindle is parallel to X-), it would work on a horizontal mill with the rotary axis parallel to the Y-axis. You might even be able to set up the rotary axis parallel to Z- but your mill will need a lot of headroom between spindle and table.

However, you specified in your initial post that you want the spindle vertical and the rotary axis parallel to X. If this is the case, then it won't work.


Offline Doc

  • Jr. Member
  • **
  • Posts: 86
  • Country: us
  • Old but still usefull (I hope) ?
    • My Youtube Channel
Re: camshaft machining
« Reply #13 on: August 15, 2019, 10:06:46 AM »
I did a V8 cam in 2 setups surface milling with a small ball endmill.