Grinding Cams - CNC program Beta test

[dsage]

The moderator is welcome to move this thread to another location. I didn't see another forum that was exactly suited to this that had the popularity of this one.

Continuing from my previous thread question "Grinding Cams - will this work"
http://www.homemodelenginemachinist.com/f26/grinding-cams-will-work-19756/

For those of you who are CNC mill equipped, we now have a properly working program that will generate Gcode to grind a cam. It properly takes into account the diameter of the grinding wheel unlike my previous attempt using modified Camcalc numbers.

We named the program Gcam and it is free to use. It's is a web-based application so you don't need to install anything. You enter your specs into the program on-line and it creates the Gcode in a file you can download to your machine. Eventually John will release the source code for it.

With this program you set up your camshaft or cam pair blank in a rotary table horizontally along the X-axis on your mill table and mount a grinding wheel fixed to the back of the machine. The Gcode drives the Y-axis into and away from the grinding wheel and turns the rotary table to control the shape. This gives you a finish ground cam exactly to the specs you choose.
(see picture in next post)

What we're looking for is some people to try the program. If you already have a CNC mill with a rotary table and you have a toolpost grinder then all you'll need to build is a mount to hold the grinder solid to the mill.

I've created a Yahoo group for the program at
http://groups.yahoo.com/group/GCam_CNC/

If the link above doesn't work the group name is Gcam_CNC

The reason for the Yahoo group is that it's easier for me to manage the pictures and users manual changes with direct access as moderator.
If you already have a Yahoo account then please join that group. I've posted a full users guide and a lot of pictures of the setup in the files and pictures section to help you out.

We already have on board Mike Rehmus from Model Engine Builder magazine and Carl Wilson who has written several articles for that magazine on grinding cams.

If all you want to do is have a look at the program and generate some Gcode to look at then the program is available at:

http://gcam.lucasemail.org/

You should really download the users manual from the Yahoo group since there are a things that need to be explained about the program.

All I want is to get it out there for comments and to see if it will be useful to you people that are equipped with CNC mills.
I've ground several cams with it and have done some checking at 16x magnification and it appears to generate cams exactly as specified with a nice ground finish.
We'd appreciate some further testing and comments.



I'd hate to have to duplicate the effort on two forums but if you want, you can comment here as well.

Thanks

Dave Sage
John L. (programmer)

 

[dsage]

Since a picture is worth a thousand words, here is a picture of the basic setup.
You'll note my nice grinding spindle driven by an old electric sander motor. Proof that it doesn't take much to grind a nice cam. The spindle is fastened solid to the back column of my mill drill with the center height of the 7" grinding wheel at the same height as the axis of the cam blank.
As I mentioned there is a lot of other important information contained in the Yahoo group Gcam_CNC so you should look there.

Sage

 

[mu38&Bg#]

Looks interesting!

 

[///]

Awesome work Dave.
I'm not at cam grinding stage yet, but after reading your previous thread I know this is going to be of benefit to a lot of people Thm:

 

[dsage]

I hope so.
But I wonder if the combination of people without CNC, those that don't have a lathe toolpost grinder they can use or those that are unwilling to make a grinding setup will doom it to failure.
On the original thread I show where I used a typical mini-grinder which most folks have around to do the job. Only a mount required. It's not as good as a proper stone wheel but it does work.

There is nothing wrong with the other methods of making a cam but it seemed to me that filing a cam even for a final finish was a bit counter productive.
Almost anything will work on a model engine but to my way of thinking why not make it perfect if your going to make it.


Sage

 

[Dave Sohlstrom]

Dave

One question and one suggestion.

Does the program do all the cam lobes on a cam automatically.?

It may be a good idea to make the Yahoo group so anyone can read the messages to get an idea of what the group is about.

Dave

 

[jwcnc1911]

This is pretty aswesome. I was just talking to enfieldbullet about making a dedicated cnc lobe milling machine and a grinder based on some of our machines at work. I think on hobby scale the cost of a dedicated machine would be more than doable - especially home built.

 

[dsage]

Hi Dave:

No the program does only one lobe. For at least couple of reasons.

Each lobe will need to be re-programmed anyway since the grinding wheel is wearing as you go.
It's just not worth the extra confusion in the program to have to program the whole camshaft with the distance between lobes since it probably varies anyway due to bearings spacing etc.
The lobe separation angle between intake and exhaust lobes is also not worth the effort and confusion for the above reasons, and, with a CNC machine it's a simple matter to manually issue a command to rotate the cam by the required number of degrees and reset the DRO to zero and start again when you're ready. The grinding always starts at zero degrees that being the tip of the lobe.

Re: opening up the Yahoo group:
I'm pretty new at managing a Yahoo group. So far I haven't seen a way to "open it up" so anyone can view the messages just by going to Yahoo groups. One still has to "join the group" to be able to look at the messages. The best I can do is make it so I personally don't have to approve a person trying to join.
But they still have to join.
A GRROUP a little bit different concept than a FORUM like this as far as I can figure anyway.
If you know otherwise let me know and I'll consider it.


Sage

 

[dsage]

Jw:

The cost is almost zero if you already have a CNC mill. (which is why we created the software). No need to make a dedicated machine when you might already have it.

I thought about a dedicated CNC grinding machine but I figured it would be about the same as building a dedicated CNC milling machine if you want it to be any good. Probably would not be cost effective. It would certainly be more than a dedicated mechanical grinder due to the steppers,drivers, computer and software etc.

Sage

 

[jwcnc1911]

I realize that adding this to your existing mill would cost less. I'm talking about a package that would take up about a cubic foot and cost around $600. It would have movable steady rests for rigidity. PM me your email address, I'd like to show you my considerations, not to mention I think my example will give you some inspiration (I machine cams, cranks, heads and blocks for diesel engines for a living). I'm thinking it could be used as a roughing mill and for grinding. Essentially you put in a blank piece of stock and get a finished cam or crank out. Plus you could generate the path with standard lathe CAM for live tooling. I think it would be kinda like a sawzall, you'd find many ways to use it. Just a thought. It's a long term goal for me any way, I figure I'll eventually get into IC even though I have basically no interest at all right now.

 

[Dave Sohlstrom]

JW

I'm not sure that I want a grinder mounted to my CNC mill. Grinding grit will make it's way to the ways no matter how much you try and keep it out.
I would think that a small machine built to grind cams and cranks up to maybe 8" long would be the way to go.
I know that there are not a lot of folks out there that would want to build such a machine.

Dave

 

[dsage]

JW:

Feel free to post a picture of your idea here but I'd rather stay on topic - which is to discuss using our new program to grind cams. I guess what I'm saying is that the machine you'd end up with to run our Gcode would essentially be a dedicated milling machine. No point in building another one that will for the most part sit around collecting dust when you are finished. This is partly why I went this route. I was too lazy to build a mechanical cam grinder when I essentially have a very precise device already in my CNC mill.


Dave:

I considered the issue with grinding "grit" as you call it. In fact there is very little to worry about. It is not thrown all over the place it stays directly below the grinding wheel for the most part.
I start by first mounting the rotary table. I then drape heavy plastic from high up under the milling head, down over the table and the rotary table and to well below the machine. I then poke a hole through the plastic just big enough to pass the cam blank into the chuck on the rotary table. I hold the plastic down where necessary with small magnets. (all of that was removed for the picture taken above).
In operation I place several of those flat magnetic fridge magnet thingy's right below the grinding wheel area. They collect most of the grindings.
Most folks are thinking that the grit is grinding stone. If things are working properly the wheel wears very little so almost all of the "grit" is metal. I don't grind hardened blanks. I harden them afterward so the grit is no harder than normal swarf.

Having said that I will warn that when you dress the wheel, that grit does fly around quite a bit. So what I do is hold a vacuum cleaner right up to the diamond dresser during that operation and it all gets sucked up. The vacuum could also be placed near the grinding wheel but my shop vac is very noisy so I choose not to use it.

So far the machine has been spotless after I carefully remove the plastic. I don't reuse it. I have felt the machine after the grinding and have not detected any grit.

To each his own I guess.

Sage

 

[ruzzie]

I did a test using a 2mm ballnose cutter and I must say it went better that expected.Their was a bit of mucking around with the code to run in the Z axis.
It was cut as if your grinding wheel was 1mm wide and your lobe is 6mm wide, you take your first cut then move across 1mm and take your second cut and so on until you covered the width of your lobe.
I will also post a more detailed account of what I am up to on http://groups.yahoo.com/group/GCam_CNC/

 

[jwcnc1911]

No problem, when I start posting my project I'll start a new thread.

What I'm envisioning will be more like a lathe with live tooling - almost anything you want to make on a lathe would be possible. Not just cams and cranks.

I actually intend to start drawing it up in the next few months. Any one interested in such PM me and I'll shorten my time frame if there's enough interest.

 

[dsage]

Thanks Ruzzie:

Even though you not grinding I'm happy to see you giving it a try. I never thought of doing it that way since the intention was to end up with a smooth ground finish. But "whatever turns you cam"
Looks the the program is going to be more versatile than CamCalc for those with a CNC miil.

And as you mentioned there is a bug in the program in that it does not accept Z as the moving axis. It should. John will no doubt fix that when he gets back from holidays.

Thanks for finding that bug. This is what the beta test is all about.

Thanks

Sage

 

[Dave Sohlstrom]

What would happen if you were to use your mill with the program to rough out the cam lobes. Then heat treat the cam. After the cam has been heat treated put it back in the machine and finish grind the lobes and bearing areas.
If you configured you grinding spindle so it would go slow enough to use a narrow diamond wheel on hardened steel. You could grind all the lobes at the same wheel diameter setting in the program. I know you can not grind steel on a diamond wheel with the wheel turning at high speed. The wheel loads up with steel and wrecks it.

Just food for thought

Dave

 

[dsage]

Hi Dave:

So far I've only used the program to generate cam-pairs for the Howell V4 engine - which I turned into a V8. The camshaft uses ball bearing races so the shaft needs to be built up from pairs of lobes slid onto a shaft along with the bearings.
If I were to create a whole shaft I would have thought it would be difficult to remove the cam from the grinding setup and get it indexed back into the grinding setup after hardening. This fear might be unfounded since a simple flat or pin somewhere would remove the issue. (read on)

We are certainly not here to dictate how to create a grinding setup, just to supply the program to generate the cam lobe shape.

Feel free to try anything you wish and report back to us.

If there is anything I have concluded about producing cams by any method it is that only a few thou of eccentricity in the lobe axis with respect to the shaft axis can cause havoc with the timing of the opening and closing of the valve from the expected results. Especially when the typical valve lash setting on a model cam are typically only a few thou. I have seen the valve open where expected in it's rotation but close in the wrong place or not at all because the lobe is (let's call it) lop sided on the shaft. So far this has come from the cam blank not running true in the chuck / collett etc holding it while being ground. As mentioned by only a few thou.

Dave Sage

 

[Dave Sohlstrom]

I'm just thinking out loud in print right now. I have never built a cam so it will be a steep learning curve.
As I said in the Yahoo group, I hope to some day build a pair of 4 cylinder engines for a model tow boat.

Dave

 

[kvom]

Where you say rotary table above, I think you mean 4th axis, since the control needs to rotate the camshaft.

 

[Dave Sohlstrom]

dsage has his rotary table set up as the 4th axis A so it does rotate the cam blank correctly.