Grinding Cams - Will this Work?

[dsage]

I'll ask this question here because I'm sure you are all aware of this method of making a cam:
Take a cam blank,hold it horizontally in a rotory table,
Rotate it a number of degrees, lower the cutter a pre-determined amount,
Take a flat cut across the side of it, turn it again, lower the cutter some more (or less), take another flat cut across it etc. etc.
In the end you have a rough cam shape with small steps instead of a smooth surface and you then file it to remove the steps.
The amount to turn and the depth of cut can be calculated from a program called CamCalc which is free.
Hopefully you know what I'm talking about.

How about this idea:
Hold the cam blank horizontally in a rotory table (as above).
Arrange a fixed grinder at the back of the milling table with a stone the width of the cam lobe. instead of a cutter (as above).
Advance the table Y axis into the grinding wheel the same amount (as above). The result being you get the flat spot in one touch without having to move across the lobe with a small cutter. No difference from above really.

Now the new idea:
Instead of backing out when you rotate, keep the wheel where it is and rotate the cam blank (as above) the prescribed amount.
BUT if you do this with a CNC machine and GCODE program you can put the rotation AND the depth of cut command (A and Y) on the same GCODE line and you'll get a (somewhat smooth move in both rotation AND depth of cut (Y) at the same time.
This should produce a smooth surface joining the individual points requiring little or no filing instead of rough steps.

Sounds reasonable to me but I can't figure a couple of things and I need some help getting this straight in my mind:

As with any outside profile milling the path taken depends on the diameter of the cutter (I think). Also I know that real cam grinders use master cams that don't look anything like the finished cams and you have to use a follower the same diameter as the grinding wheel.
In this case we have a wheel that is say 4" in diameter. Does that matter?

On the other hand the wheel is only touching the side of the cam blank at one point so does the diameter of the wheel really matter.

I need help getting this straight in my head.

I'm about to try it. I have the Gcode figured out but am I wasting my time?

Sage

 

[Jasonb]

You would treat the edge of the wheel like any other cutting tool and touch down to set a starting point.

May be better to rough out the cam first and then finish with the grinder as taking a large cut off will heat the part and wear the wheel

 

[MuellerNick]

Yes, that works. Works like any CNC Cam-grinder.
The diapeter of the wheel does make a difference.


Nick

 

[thayer]

Pretty sure that is how the Sherline cam grinder works.

http://www.sherline.com/8650pg.htm

 

[canadianhorsepower]

Yes, that works. Works like any CNC Cam-grinder.
The diapeter of the wheel does make a difference.


Nick

Hi The diameter of the wheel does or does not make a difference.
I don't think is does if your using a follower cause the ratio doesn't change


look at the pictures

cheers

 

[MuellerNick]

I don't think is does if your using a follower cause the ratio doesn't change

But he intends to use a CNC. And there too, the diameter of the wheel and of the follower have to match. Difference is, with CNC the follower is made in math.
In the picture you posted, "Ds" is diameter of the grinding wheel. You see that both at the wheel and the follower.


I don't know why my iPad made "diapeter" out of diameter. But better than diaper.


Nick

 

[mu38&Bg#]

As stated above the actual diameter of the grinding wheel doesn't matter as long as the program is properly written with tool radius compensation. The important part is to adjust the tool radius every time you true the grinding wheel. It all depends on how accurate you want to be. Plenty of engines work fine with rough milled cams filed to final shape. A simple cam shape is easy enough to program for simultaneous 4th axis motion.

 

[MuellerNick]

As stated above the actual diameter of the grinding wheel doesn't matter as long as the program is properly written with tool radius compensation.

So the diameter does matter.


Nick

 

[Jasonb]

Diameter does not matter

What matters is the distance from the axis of the cam to the cutting surface, its just like putting any tool in your mill you don't worry about how far it sticks out the collet you just touch down the end of the cutter.

 

[MuellerNick]

What matters is the distance from the axis of the cam to the cutting surface, its just like putting any tool in your mill you don't worry about how far it sticks out the collet you just touch down the end of the cutter.

I must have misunderstood the initial posting. I understood, that he wants to grind at the circumference of the grinding wheel. And then, the diameter matters.


Nick

 

[mu38&Bg#]

So the diameter does matter.


Nick

Yes, Nick, the tool radius is important, just like any other CNC process, not only CAM grinding.

Nick, you very well understand that Gcode can be written such that any diameter cutter could be used to mill a part which has no inside corners. The machine just needs to know the diameter of the cutter in order to perform the correct moves. Tool diameter, 3", 28m, whatever, is not related to the part itself in anyway in the case of the cam assuming radius compensation.

Now, it's also possible to program and use offset to adjust the feature size. In this case the radius of the grinding wheel is ignored and the offset is adjusted to achieve the correct cam dimensions. The reality is that the wheel does influence the form of the cam. However, assuming the program was written for a tool radius near what is being used to grind, the offset will only cause a small error. Writing code for a 4" wheel and using offset to correct for a wheel that is 1" or 10" without correcting for tool radius will result in a different cam form. The larger the wheel, the less influence using offset will have on the finished cam.

 

[MuellerNick]

If you are working with facets (that's what the OP described) and do not use cutter compensation but try to do it by yourself by just adding an offset to each segment … that will not work. That only works at the base circle and then it gets off. Right at the tip's highest point, you are OK again, then you are off again until the base circle.

That is also true if you use G02/G03 in the YZ-plane (without cutter compensation, would not work anyhow). Works with the base circle and the very tip of the tip radius.
The reason is, that the center of the chest radius and of the tip radius are not at the rotational axis.

If you use the setup described by the OP, with the rotational axis (A-axis) along X and the wheel's axis along X, you would have to redefine all axes on your CNC, or the cutter compensation will not work. The setup without changing axes would be a C-axis.


Nick

 

[Jasonb]

Have a watch of this

As you can see the guy does not take any notice of wheel dia, he sets the program to start when the edge of the wheel contacts a known point, the program is just set to move the cutting edge of the wheel in and out relative to the rotation of the cam.

[ame]http://www.youtube.com/watch?v=OIWyGtXEgR4[/ame]

Now if you had a known distance between cam axis and grinder axis then you would need to know wheel dia. Really depends on how you write the program and what equipment you have.

 

[MuellerNick]

Really depends on how you write the program and what equipment you have.

Well, that IS wrong. You need to know the diameter of the wheel. If it is wrong, you get distortions.
It doesn't matter if you have wear or dress the wheel and just feed in a bit to get the right lift/base circle.
If you use a follower, it has to have the same diameter (within limits) as the wheel.

If you use the multi-facets-method like in milling, but just with a wheel instead of the cutter, the wheel's effective diameter gets infinite.


Need a drawing?


Nick

 

[mu38&Bg#]

I assumed the correct spindle axis setup would be obvious, Spindle parallel to X. What I missed is that it's not a milling machine setup, it's actually a lathe with live tool and C axis. Nick is absolutely correct that CNC cam grinding is a C axis setup. Just because the Sherline setup produces a cam, doesn't mean it's what was actually designed. I don't know if the Sherline is a real C axis with polar interpolation. A wheel large enough will produce a cam that's relatively similar to the programmed part, even if it's not a real C axis. The indexed method using flat milling is essentially the same idea with an infinite radius tool, so only offset matters.

 

[Charles Lamont]

Now if you had a known distance between cam axis and grinder axis then you would need to know wheel dia. Really depends on how you write the program and what equipment you have.

Remember that the contact line between the finished cam and the follower sweeps across the face of the follower as the cam
rotates. It is the same when machining the cam. The contact point between cam and wheel only lies on the centre-line joining the cam and wheel axes at points where the cam slope is zero - at maximum lift and round the clearance arc. At all other points you are off the centreline. Unless the wheel diameter is infinite, it has a curvature. That is why the wheel diameter does make a difference.

 

[dsage]

Wow !!

First off let me thank all of you for responding. I didn't expect such a response. I think I see about a 50/50 split on whether this is going to work or not.
I spent today making the mount for my minigrinder. But I never got a chance to try it. Might not for another 3 days.
I guess a picture would be useful but basically the mount just fastens the grinder to the column at the back of my mill drill (SOLID) with the edge of the wheel in the Y direction (axis parallel to the table X) and the height so the axis of the wheel is the same as the height of the center of my rotary table.

It could be used exactly like the facet method by turning the rotory table - moving in, in the Y direction the prescribed amount according to the CamCalc program. In this case the cutter would be the grinding wheel.

What I propose to add to the process is, instead of moving the grinding wheel back out, rotating the blank and then back in to a new prescribed depth I would drive the rotory AND the Y axis at the same time by putting the new angle and the new depth on the same line of G-code.
By having the A and Y moves on the same line in the program, it is the nature of Mach 3 (or any CNC) to drive both axis' at the same time to the new location thereby blending what would normally have been steps.

No special programming is undertaken i.e cutter compensation etc. I'm using the angle and Z axis data exactly as it comes from CamCalc except I'm swapping the Z axis (depth of cut per facet) for Y - still depth of cut. And the rotory stays the same as in the CamCalc requirements.
I'm fastening the grinder to the column and using the Y table movement (instead of Z) because I couldn't figure a good way to fasten the grinder to the quill solidly. Too many obstructions.

I hope this helps clarify what I'm doing and that someone can help me figure out if these moves between facets will work.

I can't see it being much different than blending facets with a file. But then if I were sure about that I wouldn't be asking.

PS> I had previously looked at the Sherline video and wasn't sure what he was doing with the Y axis (in out). You can't really see it in the video. He doesn't say much except that "the program is very complex" and that it took him a couple of months to write it. Something about problems when you grind the peak of the cam and the axis' changing. It didn't answer my questions.
Somehow I think he's right but I can't see why. Or perhaps what I'm plannning to so is fundamentally different.




Thanks

Sage

 

[MuellerNick]

Sage, your method works, but not the way you think. It is more complicted.
Charles described it very well in words why you need to compensate for the wheel's diameter. But words can be very abstract!
I do understand where you don't understand.
Sure, you can rotate and move in/out at the same time. But the problem is, that the wheel doesn't cut where you think it cuts.
The method you intend to use is good, but it is complicated from a mathematical POV. If you would use a C-axis, the math will be very simple, but the setup gets a bit funny (tailstock).

I think I'll draw a picture tomorrow that shows what Charles wrote. I'm in bed and writing this on my iPad.

Nick

 

[dsage]

Some added information. Remember I'm grinding a model cam not a full sized one. The cams lift is only .074 and I'm using a 4.5" diamter grinding wheel. If that makes any difference in terms of an (relatively anyway ) infinite sized grinding wheel.

Sage

 

[gus]

Hi Fellow HMEM Members,

Will be bookmarking this thread as there a possibliity when my IC engine building prowess grows, four engine building can be made possible.With a basic machineshop limited by space,I can only rely on simplest methods as threaded.

Gus,now recovered from food poisoning last nite. I was one of the 200 at a function.Sure great to have a Nursing Officer as wife.