Two sided machining

This forum is for general discussion regarding VCarve Pro

Re: Two sided machining

Postby martin54 » Wed Apr 03, 2019 12:43 am

I only started plugging my leftover alignment holes to stop my confusion. When I get do a lot of double-sided machining, I lift the project to flip it..... and have to figure out which set of holes match.. :oops:

You need to sort your jobs out so some of them use the same sort of size board, that way you can use the same set of holes for multiple jobs :lol: :lol:

Maple and so to get a dimensional lumber 8" wide would require a 1" X 10" which would get very pricey. All of my results have been close but not close enough when CNCing. My last attempt I made a two sided jig square to 90 degrees. My material is square. So I centered the bit in the corner of the jig. What I forgot was the bit is 1/2" so I needed to be 1/4" further on x and y. In the tutorial they make mention of zeroing z on both sides of the material. So if the material is square, and the thickness is the thickness, once you have your set up why would it be necessary to reset any axis. The material is the same thickness from both sides? If, and I say if, your set up of the bit is correct, with the jig in place this should be repeatable. Now that's my thinking but I have been unable to produce it in the flesh.


It doesn't need to be 8" wide as long as it is long enough to fit the dowel holes in at the sides of the material it would probably be OK :lol: :lol:
The reason for the tutorials setting the z zero from both sides is because wood is rarely the size it claims to be so you would need to measure it accurately & use that figure in your job set up. Same goes for the wood being square, if you have a way to accurately size & square your timber then there shouldn't be a problem using a jig, I generally use the dowel method so I don't have to spend time making sure my material is absolutely correct. I am not actually sure I have the tools to do that :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 4629
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Two sided machining

Postby gkas » Wed Apr 03, 2019 1:14 am

martin54 wrote:I only started plugging my leftover alignment holes to stop my confusion. When I get do a lot of double-sided machining, I lift the project to flip it..... and have to figure out which set of holes match.. :oops:

You need to sort your jobs out so some of them use the same sort of size board, that way you can use the same set of holes for multiple jobs :lol: :lol:



You mean GET THAT ORGANIZED?? :shock:
User avatar
gkas
Vectric Wizard
 
Posts: 452
Joined: Sun Jan 01, 2017 3:39 am
Location: Southern California
Model of CNC Machine: Aspire, Axiom AR8 Pro+, Axiom 4.2W Laser

Re: Two sided machining

Postby jfederer » Wed Apr 03, 2019 3:57 pm

I've used both jigs and dowels. Dowels are accurate, jigs... maybe. After I do a run, I mark the dowel holes on the spoil board with a pencil mark so I don't have to guess which to use for the other side. I've used symmetrical dowel holes, and non-symmetrical. They both work fine, as long as I remember to allow for tool clearance. Another "learn by near-oops" incident, I'm afraid! I of course leave the XY settings, but re-set Z. Even though I measure and set for exact material thickness, I find boards vary enough that it's just simpler to reset Z.

In short, I recommend using dowels.
Joe Federer

www.fabrikisto.com
www.federer.ca
User avatar
jfederer
 
Posts: 37
Joined: Tue Nov 27, 2018 1:09 am
Location: Horton Township Ontario Canada
Model of CNC Machine: CanCam D23M

Re: Two sided machining

Postby rscrawford » Wed Apr 03, 2019 5:11 pm

Most of the work I do is two sided. I ALWAYS use dowels to position for the second side.

There are too many ways to get an error using the sides of your workpiece to reference for the flip. And every error is doubled in a two sided cut, so it really stands out.

And I always use 4 dowel holes rather than two.

If your gantry is out of square, or if your spindle is not exactly trammed, or if your Z-axis is not exactly orthogonal to your gantry and table, then the two sides of your cut will not line up even using exact dowels.

It is rarely a software problem, unless you have a problem with your vectors. If you simple cannot get your machine set up accurately enough for two sided cuts, then you can compensate by 'nudging' your vectors a little to get the two sides to line up.
Russell Crawford
http://www.cherryleaf-rustle.com
User avatar
rscrawford
Vectric Wizard
 
Posts: 947
Joined: Mon Jan 17, 2011 6:49 pm
Location: Wetaskiwin, Alberta
Model of CNC Machine: CAMaster Cobra 408 ATC, ShopSabre IS408

Re: Two sided machining

Postby ironspider » Tue Jul 23, 2019 1:47 am

So on the "asymmetric" dowel setup how is that done exactly? In the two 2-sided videos they don't seem to actually show it. So, let's say you have a rectangular workpiece that is (X)7",(Y)5" at (Z).5" thick.

Is it correct to say that in the symmetric dowel setup you would place a dowel hole at Y2.5 (which matters) and let's say X0.5 (doesn't matter) and you are going to flip it on the Y axis. You then create a mirrored copy of that dowel hole and "flip it about job center" in the horizontal (x) right? So you then have two dowel holes in the exact center of Y and the same distance in from the outer edge of X (or I guess you could say from the same distance out of the center of X). You then drill out the dowel holes to some depth like .75" or 1" and when you're done cutting that side you place the dowels in the spoiboard holes and flip the workpiece on Y and put the dowel holes on the dowels sticking out of the spoilboard and run the bottom toolpaths and you should be good to go since the X and Y of your machine never changed correct?

So how does the asymmetric method work? You put a dowel hole at say Y1.0, X0.7 and then another one at say Y3, X6? And then you drill them out say .4"? Then, you mirror those to the bottom side and cut them into the spoilboard and then put the dowels into those spoilboard holes and sit the workpiece's .4" holes on the top side onto the dowels?
ironspider
 
Posts: 12
Joined: Tue May 28, 2013 9:23 pm
Location: Los Angeles, California
Model of CNC Machine: CNCRouterParts PRO4824

Re: Two sided machining

Postby TReischl » Tue Jul 23, 2019 1:38 pm

Dowel holes work for me, all the time.

Yesterday I used the fixture method. That works too but you have to pay attention and the fixture needs to be designed correctly. A fixture that only uses two perpendicular edges can be a problem. If it only uses two edges for location the stock had better be exactly to size and every piece must be exactly the same.

I use the fixture method when I have already cut the stock to size and can measure it precisely. Two opposite edges must be trapped in the fixture. The perpendicular edge must be located against the same edge when the piece is flipped. When flipping the stock it must be flipped over one axis only and that axis must be the one for the trapped sides.
"If you see a good fight, get in it." Dr. Vernon Jones
User avatar
TReischl
Vectric Wizard
 
Posts: 2864
Joined: Thu Jan 18, 2007 6:04 pm
Location: Leland NC
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset

Re: Two sided machining

Postby martin54 » Tue Jul 23, 2019 3:42 pm

The main differnce between using symmetrical dowel holes & asymmetrical dowels is the flipping of the material for the second side. With a symmetrical pattern it is possible to flip the material in the wrong direction but with an asymmetrical dowel pattern it can only be flipped one way :lol: :lol:
Most of the tutorials use a 3 dowel pattern.
Place you dowel holes on the first side of the design & then select those vectors, right mouse click & copy to other side, no need to try mirroring s copying to other side will take care of that for you :lol: :lol: :lol:
User avatar
martin54
Vectric Wizard
 
Posts: 4629
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Re: Two sided machining

Postby ironspider » Tue Jul 23, 2019 3:46 pm

Can you give me a link to one of the tutorials that uses the 3 dowel method? The only one I see in the Cut 2D tutorials is the cube one that uses 2 (symmetric) dowels (even though it talks about the asymmetric method). Thanks!

martin54 wrote:The main differnce between using symmetrical dowel holes & asymmetrical dowels is the flipping of the material for the second side. With a symmetrical pattern it is possible to flip the material in the wrong direction but with an asymmetrical dowel pattern it can only be flipped one way :lol: :lol:
Most of the tutorials use a 3 dowel pattern.
Place you dowel holes on the first side of the design & then select those vectors, right mouse click & copy to other side, no need to try mirroring s copying to other side will take care of that for you :lol: :lol: :lol:
ironspider
 
Posts: 12
Joined: Tue May 28, 2013 9:23 pm
Location: Los Angeles, California
Model of CNC Machine: CNCRouterParts PRO4824

Re: Two sided machining

Postby martin54 » Tue Jul 23, 2019 10:32 pm

Try these for now, there are other tutorials that cover this but I will need to look for them, unless someone else posts before I can find them :lol: :lol: :lol:

https://support.vectric.com/tutorials/V ... =2%20sided
User avatar
martin54
Vectric Wizard
 
Posts: 4629
Joined: Fri Nov 09, 2012 2:12 pm
Location: Crossgates, Scotland
Model of CNC Machine: Gerber System 48 (modified)

Previous

Return to VCarve - General

Who is online

Users browsing this forum: martin54 and 28 guests