[FoxCNC1]

Hey guys, I want to make some two side parts, and I am wondering what is the workflow for this.
I have noticed that much of it comes down to centering the part along the flip axis?

Some advice would be appreciated.

[awerby]

Here's one way to do it: set up the drawing so that the X, Y and Z zero points are in the middle of your part. Make a spoilboard with a couple of pins sticking up well outside the part boundary. Drill the workpiece with holes corresponding to the two pins, then set it on the spoilboard and clamp it down. Zero your tool in the middle of the part, carve the first side, then unclamp, flip, reclamp, and carve the other side.

If that's too complicated, DeskProto has a "two-sided wizard" which makes it even easier; you set up right angle blocks on the corner of your part, and take a cut on the back edge (as directed) so that you can flip it over without losing registration.

[FoxCNC1]

Thank you, I was thinking something like that too.
What I did as a test was to bolt the part to the spoil board, cut one side, then flip and cut. I had zeroed the bit one one corner, but what I think is important is to flip the part perfectly along its center.

This is where the spoil board with the pins comes in handy I think.

The only challenge becomes when you have to cut different 2 sided pieces I would think (different size stock)

[Spk64]

My technique for 2 sided routing is add 2 fixture holes in my stock out side the normal part.
1. Create a file to just add the holes in a sacrificial board.
- the X Y zero is left fixed for subsequent operations
2. Clamp/secure workpiece to the sacrificial board
3. Run top side machining along with the extra fixture holes
4. Flip part over using fixture pins to align part.
5. Complete back side machining.

Everything remains perfectly aligned and your same zero is used.


Steve

[FoxCNC1]

My technique for 2 sided routing is add 2 fixture holes in my stock out side the normal part.
1. Create a file to just add the holes in a sacrificial board.
- the X Y zero is left fixed for subsequent operations
2. Clamp/secure workpiece to the sacrificial board
3. Run top side machining along with the extra fixture holes
4. Flip part over using fixture pins to align part.
5. Complete back side machining.

Everything remains perfectly aligned and your same zero is used.


Steve

Steve,

Thank you for sharing. I am guessing that once you cut the hole of the sacrificial board you leave it attached to the router table and not move it.
Then you attach your stock and cut your part as described.


I wonder if I could build the registration holes right into my top surface to be able to cut a 24"x24" sheet. I guess that I would need to home the machine and offset to a work offset that lines up with the existing registration marks. Does that make sense?

BTW, here is a visual of what I understood your process to be, correct me if I am wrong:

[Spk64]

You have it except keep the holes centered and not in opposite corners. Then when you flip the part holes are where they need to be and part is mirrored.

Here is an example part.
First side
Attachment 227222
Second side
Attachment 227224
Steve

[Spk64]

Steve,

I wonder if I could build the registration holes right into my top surface to be able to cut a 24"x24" sheet. I guess that I would need to home the machine and offset to a work offset that lines up with the existing registration marks. Does that make sense?

This would work, but if your work pieces vary greatly like mine you are always trying to force a fit or add new holes.

My main table is aluminum jig plate with dowel and bolt holes. When I home my machine I know exactly where the dowel and bolt holes are located. With this I still find myself just using a sacrificial board and adding fixture holes.



Steve

[FoxCNC1]

got it, so you basically make 4 holes.

My main table is aluminum jig plate with dowel and bolt holes. When I home my machine I know exactly where the dowel and bolt holes are located. With this I still find myself just using a sacrificial board and adding fixture holes.

I see, well I guess that if you need to cut a 24x24 stock, you will need a 24x24 spoil board every time.
BTW how does one go about getting a table top like yours? It seems like nothing gets better than that and I like how you lift the work piece so that you don't cut into the table.
I thought of getting 80/20 for mine, but yours seems much better

[Spk64]

4 holes total. 2 in the sacrificial and 2 in the stock.

I built my top using my cnc router.
1" thick MIC6
Machined all edges, bored all dowel holes, Cut all the threads on the cnc router.
Top also has a manifold underneath to attach a vacuum source. I have presently been using 1/2" MDF over the aluminum table and vacuum as a hold down for my parts.
Here is a shot of the vacuum hold down. 3/4" MDF cutting full depth with 1/4" cutter.



My build thread showing more details on the table top.
http://www.cnczone.com/forums/diy-cn...nc-router.html

Steve

[FoxCNC1]

impressive work. thank for the link.

[FineLineAuto]

Typically, there are 2 easy ways to do this. The easiest is to put 2 pin holes in your spoilboard, and locate the piece of of 2 pin holes on the workpiece. This allows you to machine the pin holes on the first side and then when you flip it over your references will be know.

The second way is useful if you have standard shape parts like squares or circles. You would mill the outer profile on the first side of machining. Then, you would put 2-4 pin holes in the spoil board. These holes will accept pins. When you flip the part around, the edges of the part are located against these pins and thus in a repeatable position.


Nate
Fine Line Automation
Home - Fine Line Automation

[FineLineAuto]

Typically, there are 2 easy ways to do this. The easiest is to put 2 pin holes in your spoilboard, and locate the piece of of 2 pin holes on the workpiece. This allows you to machine the pin holes on the first side and then when you flip it over your references will be know.

The second way is useful if you have standard shape parts like squares or circles. You would mill the outer profile on the first side of machining. Then, you would put 2-4 pin holes in the spoil board. These holes will accept pins. When you flip the part around, the edges of the part are located against these pins and thus in a repeatable position.


Nate
Fine Line Automation
Home - Fine Line Automation

I have no clue why this response got posted 2 days late... The others have pretty well explained it.


Nate
Fine Line Automation
Home - Fine Line Automation

[tinygiants]

http://www.cnczone.com/forums/diy-cn...ml#post1338118

The above link is to a build thread here. At the bottom of that post, is a video of him doing a 2 sided milling. His method of fixturing is pure genius. Platform CNC | Milling a Two Sided Soap Dish - YouTube

Dale

[FineLineAuto]

Man, I would have never thought to do it that way. That is way too cool. I am definitely gonna borrow that idea.


Nate
Fine Line Automation
Home - Fine Line Automation

[FoxCNC1]

I tried this last night and it works well. Not sure for larger parts though.

But yes. Great workflow.

The edges of my flip geometry don't line up like this though.

[FoxCNC1]

anyone give the method on the video a try?
it works pretty well. I was able to finally make some double sided clamps.

It take some time to set it all up digitally. But its very easy and work - less error I think.

I did notice that with any workflow you still have to manually think and manage the mirroring of the toolpatht etc. depending on how you are going to flip your part.

[FoxCNC1]

Hey guys, I have been trying some 2 sided parts recently using the dowel method we all have been discussing but for some reason, when I cut the "back" side, I seem to be slightly off in the Y direction. I do not think my machine is losing steps or anything like that since all the part features seem correct to 0.005" which is acceptable to me. There is a shift of 0.02" in my part after the flip and I think this may just be the margin of error of manually doing the flip.

I am only zeroing my machine once on an edge of the stock. I was thinking that maybe I can create a feature that will allow me to zero the router on the flipped stock in order to get better results?

any thoughts or advice?

[Spk64]

Not sure of the size of the part or where you are seeing the mismatch but any errors in your machine will be doubled when you flip the part.

So if it is .010 out of square in a given length, it will be .020 mismatch when flipped.


Steve

[ger21]

Also, if your dowels are in the center (flipping axis), your zero position must be an exact distance from the dowels. Zeroing to the edge will almost always give you an error.

[FoxCNC1]

Good morning guys,

I only zero once at the beginning, but in my example I would zero the second time to a point in an already cute and flipper feature (U would need a way to find that point on the part accurately but that is in the works).
My machine is of 0.003"-0.005". Which would mean that when I flip I am off 0.01".

So are you suggesting that I need to have a machine with "ultra" precision ? (0.000)

But what doesn't make sense if that all the feature of both sides are the proper size... I'll have to do more testing.