[CNC] CNC from sketch to part the way I do it

It has been awhile since i have added anything to this thread and I finally have a project I think will be interesting and challenging to add.
I was recently contacted by Bill Gruby about assisting him making 2 parts for his 18 cylinder Radial engine build.
( ADD Bills thread here )
I was a bit puzzled by Bill's request because if any of you know Bill he is very interested in Cnc but honestly doesn't need it to accomplish
the many things he builds and shares here in the forum. I have yet to see anything he could not make and was sure he could make these parts.
Bill mailed me the prints for the 2 cams for the engine and the directions for machining them manually that were included with the plans.
The challenge became immediately apparent as I read the directions and imagined myself trying to follow them and what my end results would have been.

To just machine out the cam lobe profiles on on the rotary table there would be 280 separate 1 degree moves of the rotary axis and the Y axis that
have to be at the same time, meeting at the same end point to ensure a good finish. you would have to keeps in mind the machines backlash and reset the dial to zero for each change in y axis direction.
that is a .001 to .003 move in y and 1 degree of table movement 280 times to complete 8 cam lobes. and there are 2 of these cam rings.
If you tried to move one axis then the other the finish on the part would be a series of very small steps around the entire profile that would need to
be finished smooth by hand when done.
reading each line of the directions then preforming the move without any mistakes and not getting a headache would be beyond anything I have ever done.
one mistake and the part is scrap and there are 2 of these that need to be exact to run right.
anyone who knows 4 stroke engines and the effect of any changes to a camshaft have on performance would see the problem here.
these cams can be made and the motor will run but the difference is in how smooth and steady the motor runs can very a lot.
this is a real determining factor in how all the work to everything else made comes out in the running of the model engine.
So with all that said how will I do this on a Cnc 4 axis mill is the next question and the answer was not as easy as I expected.
there are different types of 4th axis functions and most wont work for this part.
In most 4th axis setups on a Cnc mill the rotary axis is mounted standing up facing the z axis from one of the four opposing directions available
X+ X- Y+ and Y-.
Different types of cam software's do different types of operations from different locations of z to the axis. z axis centered behind or in front of the
center of the rotary axis is used to make things like gears.
for my examples the rotary axis is mounted on the left side of the x axis facing z.
for the setup I just described the x axis moves back and forth as the y axis increases the depth of cut and z doesn't move.
when each operation at that location completes y backs out from z the the rotary axis turns to the next location and repeats the operation.
this is 4th axis indexing and can be done with z above or to the side of the center of the rotary axis.
This operation will not work for a cam lobe.
the next type of 4th axis operation is called wrapping.
wrapping takes a drawing that is in x y plane and converts all the y or x moves ( determined by the rotary axis location )
into rotary axis rotation at a given circumference. if the y or x axis length 2" then you will wrap that around a circle with a circumference of 2".
z is lowered on each line and follows it at one set depth. raising and lowing to cut each line.
This will not work to cut a camshaft.
the next type of rotary axis operation is rotary axis turning. in this operation the rotary axis rotates and the cutter removes material at a set z depth,
like a lathe operation.
this won't work for a cam lobe.
the next operation is rotary axis contour turning
in this operation the rotary axis rotates and the z axis moves up and down and the x axis side to side as the part is rotated
this can make a cam lobe but only with a ball end mill and the finish would be a series of lines around the cam as the cutter moved in x direction.
this would be smoother than hand making the part and more accurate but would still have to be hand finished.
you can't cut the profile in one pass with a flat bottom end mill eliminating the ridges a ball cutter would leave because the flank side of the cutter
as z moved down would cut
into you lobe as it lowers.
If I did do it with the ball end mill and decided the finish would be acceptable to polish out, the end mill would have to be less than an 1/8" because the
cam lobes in each row are that close to each other.
this will not cut bills cam to the desired result.
so to do this with a standing rotary axis to a close to desired result the y axis will have to move also so the cutting surface on the flat cutter moves
from center to flank as the z axis lowers and face to center as the z axis raised and the cam lobe rotation crosses center. since the
face and flank shape of the cutter contacting the lobes will be concave and the lobe would have to be cut by stepping in from the side in small increments
to keep from leaving lines like the ball end mill.
this software for for this type of 4th axis operation is very expensive and I don't have it.
this is Not an available choice for bills camshaft from me.

Since 2006 I have tried demo software's whenever available and I have never seen the 4th axis operation I need for this project
I want to cut with the side of the cutter so the cutter will not leave lines around the circumference. one finish pass at a set depth from start to finish.
to do this the rotary axis has to be mounted on the mill table facing up centered with z axis and all the moves to make the lobes have to cut in
either y or x direction away from zero.
the reason I haven't seen this approach to rotary axis is because a Cnc milling machine can cut this shape without the need of a rotary axis. by moving x and y in any direction
it can cut any shape. makes sense right.
well not for Bills cams.
on Bills cams as your looking down on the print there are undercuts that come in from the sides with the part mounted in this direction.
the cutter has to step in from the side below the upper cam to cut the lower cam.
I'll have to cut this from the side with a Woodruff key seat cutter.
problem solved? well almost. true I can set the z height to the correct cam lobe height then with the software I have move in and cut the cams Outside diameter by moving the x and y axis until I have moved all the way around the part, lower z and repeat for the next cam shape.
then move out and up to clear the upper lobe.
a little hand coding and it could be done that way.
well not with my machine and mach3.
mach3 backlash compensation works perfect in a linear move but has trouble working in an arc. I have .0015 backlash in x and in y.
the end result will be four or more bumps in the surface of the cam where mach3 compensated for the backlash.
where to go from here...
I have it figured out and I know how to accomplish what I need to do but I'm tired of typing and will post how I'm going to do it and show what I am doing in another series of posts with pics and maybe videos .
Thank you for viewing
Steve
 
Last edited:
here is a photo of a cam and the followers in a radial engine and two pics of the plans I have
the pics are blocking certain parts because they are copyrighted and are here for just an example.
these are plans and not cad files so in order to machine these parts in a cnc mill i have to draw them
exactly to spec and make the g-code from my drawings.
to start with I need a top down view of each cam with all 8 lobes, intake and exhaust. there is a front and a rear cam so that is 2 drawings like these.
they will be used to rough away the material from the top down in conventional cnc milling.
sometimes you can copy a print and trace it into a cad program to get what you need but this will not work from
these drawings because they are copies of copies and the lobes seem to be hand drawn.
so I have to draw from measurements.
the plans have location measurements for every degree of angle and the distance from center for that point including the radius of the Woodruff key seat cutter.
so I have everything I need to draw these cams.


DSCF1813.JPG DSCF1834.JPG Radial EngineCamshaft and Follower.jpg
 
Last edited:
this engine has 9 cylinders per bank front then 9 rear, 18 total
there are four cam lobes for the front nine cylinders intake and 4 exhaust. that means that each time the crankshaft turns 2 rotations on number one cylinder, the cam is on the next set of lobes for number one cylinder. there are 4 sets of lobes so the engine rotates 8 times before it gets back to the original set of lobes for number 1 cylinder.
with 2 cams and 18 cylinders the engines fires 9 cylinders every revolution.
that part has nothing to do with cad or cnc but was just too kewl to not mention
Steve
 
I noticed in the directions to mill this part manually that the cam lobes have the same shape on their approach to cam follower as leaving the cam follower. this means that once I have drawn one half of one lobe the reverse side is a copy flipped over and rotated into position.
that will complete one lobe. I Then copy that completed lobe and rotate it 90 degrees and that the next lobe. i copy the last lobe made and rotate each 90 until all 4 lobes for the circle are done. I then connect each lobe with a line on a 1.5 radius and I have the complete intake cam drawn. the exhaust is done the same with its measurements.
I tried that first that is the machining path of the 1/2" cutter not the drawing of the part.
I could use this to cut the part out and it would be right but it is not a cad drawing of the part it is the path the tool needs to follow . For my needs
when I rough out the part I want to leave .005 clearance by telling D2nc that my .500 cutter is .510. this will leave .005 around the entire part for a finish pass.
so shorten the lines by .250 because the cutter is a half inch and and then connect the tops of all the lines right. that removes the cutter.
no, that will draw a lobe but it does not include the tangent of the cutters edge contacting the material as it turns it shows only the y axis point of contact.
in order to draw the correct shape of the lobe I had to draw all the lines extending out from 0 in 1 degree increments. place a .5 circle on top of each line and intersect the tangent of each circle to the one next to it. delete everything else and the tangents are the true cam lobe and the shape the cutter will leave.
I hope these pics are in the right order.
Steve

DSCF1814.JPG DSCF1815.JPG DSCF1816.JPG DSCF1817.JPG DSCF1818.JPG DSCF1820.JPG DSCF1821.JPG DSCF1822.JPG DSCF1823.JPG DSCF1824.JPG DSCF1825.JPG DSCF1829.JPG DSCF1830.JPG DSCF1831.JPG DSCF1832.JPG DSCF1833.JPG
 
Last edited:
photo number seven shows 2 circles one red overlapping the first drawing.
the circles represent the cutter and if you notice in the red circle there is part of the first drawing. that is why i had to use the tangents to draw the lobe.
the material would not have been removed following the first drawing and did not represent the true cam lobe shape.
Steve
 
Once I had the cam profile drawn I made this video to show how I produced the outside contour roughing g-code
Thanks for viewing
Steve

 
Here is another video, this one goes into the d2nc cam software and then to mach3 with the drawings I have made in the previous video.
If anyone has anything to add, comment on, or critique please do. I'm not an instructor on any of these software's but that is probably why no one is doing this. they think they have to be. I make mistakes and find corrections... I hope this helps get someone else started.
If i'm learning by my mistakes I have to be a genius by now... lol
I get the impression from what I read that quite a few people think they need complete training on their cad, cam and operating software from a college or online course to do this and my point is for me it is easier to learn as I go.
A quote from Einstein I like is something like this " don't waste space in your brain memorizing anything you can look up "
If you have any ideas what to go into next, let me know, if there is none I guess I'm done for now.
thanks for watching
steve


[video=youtube;VXizFzP6rAw]

note: sitting in a quiet room and talking to yourself for an hour is a weird feeling, try making a video.
For someone who is not an instructor, you do a awesome job! I use SolidWorks now but have used a number of 2D drawing CAD packages in the past including Vellum, AutoSketch, various versions of AutoCAD, and Daftsight. eMachineshop looks as it would be far easier to learn. I will pass on the recommendation to anyone looking for a good CAD package and the recommendation to catch your YouTube videos. Thank you for sharing!
 
Thank you RJ
in this video I try to explain how the hand code is written to come in from the side and cut the cam profiles.
I st-udder and stumble as the squirrel in my head trips over my tongue but I make it through and I hope you can understand what I'm doing.
the video flickers this time, I just did the video before this one with no problem.
hopefully you can follow along, these are not easy to record without something going wrong.
Thanks for viewing
Steve


 
I'm on hold on the last project waiting for the materials so I have started a new project for a friend of a friend
These parts will be for the tail rotor of an RC helicopter.
I'll try to document everything from start to completion of the machined part itself.
I make a lot of mistakes and there are changes as I go along but I hope it is helpful for others.
These are not how to videos but more how I'd do it videos, and suggestions or alternative ideas are always welcome.
I'm looking for a way to make a video of actually machining the part in fast forward so i can show the entire machining process.
I had to use the same thumbnail for a couple videos because YouTube was messing with my upload, but they are different in content.
Steve






 
In video 36 at 2:45 in I set the depth of cut to .6 for the side view op , that is a mistake. the depth of cut should be around .385. I'll correct in the final g-code but I'm not going to make another video of it.
Steve
 
Back
Top