Is this the right way to do two-sided CAM?

[jacobcanady]

I spent a couple hours this afternoon trying to figure out how to set up two-sided machining, and I think I've gotten to a point where if I were to run the job in some stock, it would pop out a completed part.

So, let me know if this is a "correct" method:

1. Create two CAM setups, with identical stock.  For the top of the stock, set the origin wherever you want the origin to be.  Then flip the model over the same way it will be flipped on the CNC machine, and put the origin in the same location on the second CAM setup.  So for me, I put the origin at the bottom left corner of the stock, using a stock point.  When I flip the stock over (like reading a book...side to side, not top to bottom) I put the origin in the same location...bottom left corner.  

2.  Create toolpaths under the corresponding CAM setups.  In my test run, I did a pocket clearing for both.  So on the bottom, the toolpath will essentially mirror what happened on the top.

2a.  Set the correct bottom height!!  This was the key for me.  I tried using the origin, but it gave me an error, so I offset the bottom height to put it in the middle of the stock.  In my test project, the model is 6mm thick, so I offset the bottom height by 3mm, for both pocket clearings.  (And for any other toolpath I'll generate)

3.  (Haven't done this part yet)  Post process.  I'd assume you'd want to go in and edit the G-code, so that you put an M0 between each pocket clearing so you know when to flip your stock over.

Things I haven't done yet, but I probaby should:

1.  Add fixture location to the stock.  I just put some MDF over the t-table on my machine today, because I wanted to have a consistent place to mount stock for projects.  I figure it wouldn't be a bad idea to add this fixture point to any project, so the machine knows not to run into any screw/wingnut that might be sticking up.

2.  I had something else I think, but I forgot.  So...any suggestions for what consists of good practice when doing two-sided machining?

Overall, does this process seem sound to the experts?  Am I missing anything?  If you want to take a look at the test run I did, I'd be happy to post the file.

[LibertyMachine]

It would be nice to see the file, I always like to see other people's work.

One thing that would concern me, in regards to the actual locating: Having the locating point remain at the bottom left on both ops might very well cause you some grief.

Lets think about this for a minute.

If you have a block that is 2" x 2" and you want to put a hole smack dab in the middle.

You do your edge finding, set your datum. Except, you are .005" off in the "X", for whatever reason.

You cut the feature half depth.

Flip it over and locate it against the stop.

Finish the other half depth.

Now you have a .010" step between the 2 cuts.

Not certain what your machining experience is, so forgive me if I'm preaching to the choir.

For Vise work, I prefer the top left side for a couple reasons: It's up against the solid jaw, so if there is variation in material size, it will always be the proper dimesnion, in regards to the vise.

The left hand side, well, I guess it's just what works better for me when I load a part with my right hand and lock down the vice

[jacobcanady]

I don't have a ton of experience with machining...I've done a bunch of jobs with my little machine, but haven't really delved into the two-sided stuff, so you're definitely not preaching to the choir. I hadn't though about getting the centering holes perfectly centered!

I've attached the file, but Fusion just got weird on me.  When I expand the browser, nothing shows up.  Not really sure how to fix that, but it let me export the file so if it shows up on your system awesome.  If not, I'll try and get mine working properly again.

Now, actually locating the stock aside...is this typically how you'd set up a double-sided project in Fusion?

When it comes to actually locating the stock, I'm not sure I understand the difference between the top left and bottom left of the stock.  To me, setting either point as the origin would be the ame wouldn't it?  You'd still be flipping the workpiece around the y-axis, right?  (I'm sure I'm missing something here, so please don't assume you're preaching to the choir...I'm here to learn!)

[LibertyMachine]

There are 2 ways to do "2 sided CAM".

You can do one setup, establish your datum, program your first depth pass, program your second one but use Tool Orientation and select the backside face. The problem with that is this: If your Z zero is the top of the part and it's 1" thick, the first cut will be going to Z-.50 and then the second pass will be going to Z.50, which is a positive value.

The other way to do it is to have 2 setups, with the datum established as you would have it.

Of course, if the part and cut is completely symmetrical, you could just copy/paste the first section of code and insert an M0 where needed

[LibertyMachine]

where you set the datum is almost always user preference, although there are some cases where it does actually matter. It has no significance on programming it. Just know where they are and document it, so when you go to setup the job, you establish locations properly.

[LibertyMachine]

Your file opened up just fine. How you have it set is pretty much what I would be looking to do if I needed to approach a part from both sides in relatively the same setup

[jacobcanady]

OK, so the programming is sound, that's good to know.  The process makes a lot of sense to me...one of those things that just clicks!

Now getting the actual location perfect...that's the hard part.  Do you (or anyone else) have any tips or procedures for getting the stock lined up perfectly?

One concern I have is that sometimes Mach3 and my machine freak out/miscommunicate and my offsets sometimes get all wonky.  Has only happened a couple of times in the last 6 months (though today I had a weird z-axis issue).  

I can't think of a good way to get the actual setup perfect.  I'm going to use the machine to mill holes in the MDF for screw inserts and definitely will write down those coordinates.  But what is the best way to set up the stock to get it absolutely perfect?  There's got to be a better way than just measuring the stock and marking where to drill mounting holes.

[jacobcanady]

OK I think I've come up with a decent solution that *should* be perfect...or at least, as perfect as the machine.

So.  Clamp the stock down at the middle of each edge of the workpiece.  Then write a program to drill holes through the stock and into the spoilboard at the corners all equidistant from the corners, and use one of the holes as the origin.  Plug holes with dowels and run side one of the project.  Then, flip the workpiece over, line up the holes by plugging them with dowels and clamp.  Run side two.  This should produce a perfectly aligned piece because all the holes are exactly the same distance away from the corner, right?

Then you can set up that fixture offset in Mach3 and use it over and over, using the same stock fixture setup in Fusion 360, yes?  Is there a way to save that drill pattern as a template of sorts in F360?  (would make future projects much easier)

And for a future project...I could theoretically just situate the stock over the dowel holes in the spoilboard, clamp it, and run the drill program.  Even if it isn't perfectly situated, the holes more or less represent the edge of the tool workspace and create a perfectly aligned workspace, I think.  Then repeat the process all over again of plugging the holes with dowels and running side one, flip, then side two.

Am I missing something?  Or would this be a decent way to run a job?

[broncomech]

First I am also just learning both Fusion and operating a CNC machine, I have several years on a manual set up.

 For me the dowel option would be fiddly, alignment will be critical as all of the dowels have to engage equally or the part will bind before you get it seated and clamped to your fixture.

I would try to build a fixture plate that uses some sort of stop to locate one X and one Y edge against and clamp the stock in position, would be quick and simple to flip for opposite side operations.

 I do not see any tabs in your set up. For the geometry you have and the way I am understanding your setup you need some way to hold the part or it is going to end up flying across the shop as the last of the base material is cut.

[jacobcanady]

Yep, no tabs in this one because it's basically a test run to figure out the basics behind two-sided machining.  My other projects do have tabs to keep the part from flying across the room.  Good catch though, thanks!

I also like the idea of a fixture plate.  Even something like a simple bracket from home depot would work.  My concern with that is that then you need to get the model exactly centered in the stock.  Not difficult in Fusion, but it seems like you could also mill out holes that exactly fit the wood dowel method.

With the wood dowel method, the part wouldn't need to be centered because of the dowel hole being used as the origin, right?  The hole/origin would automatically center the program for flipping I think..?  Or would it still need to be centered...shoot, I don't know.  I always have a hard time visualizing this kind of stuff in my head!

Waaaaaaiiiiit I'm an idiot, can't you center the model in the stock in the CAM setup?  I think that's how to do it...which means a fixture plate (bracket from home depot) would be the easiest solution for sure!

[broncomech]

Here is what I had in mind. You can indicate the corner of your stock and save that as an offset on your machine for the job, once set you are good

as long as the fixture plate is not moved.

[jacobcanady]

Oh, OK I see what you mean.  There are several ways of achieving that then, yeah?  I could machine a piece like that and secure it to the spoilboard, or make a cut directly into the spoilboard...or just use some sort of edging to create the fence.  

How it's done isn't as important as centering the model in the stock, correct?