2 sided carve doesn't meet in the middle?

I am trying to have my Onefinity carve a violin neck/scroll. I am using Fusion 360 for the design. I’m carving it from 2 sides that are supposed to be symmetrical. It carves the first side good but when I turn the stock over to carve the side two and re-zero everything the two halves which should meet at the mid-point/center line. It does not meet in the middle.
Any ideas where the problem may be. I have pins in the spoilboard for registration. It is close to matching but not quite.

Hey Stradibarrius,
Have you tried zeroing your piece from the center in fusion?
If you are calling your material at 4" (in your model) and it is actually 4.02" or 3.98"
it will have an offset when you flip it over if you are zeroing from the lower left corner. Just a thought!
Cheers,
Neil

2 Likes

Thank you for your thoughts and help. I am not sure what you mean by zeroing in the center. Also I don’t understand what you mean by the offset and the numbers
Here is a photo of side 1 before I turned the piece over to carve side 2

Also this is just some scrap so as not to waste my expensive wood

I don’t use Fusion. Most programs that you are going to use to model will let you choose where you want to have your router start from. Most people use the lower left corner of their work piece. You should have the option of any corner or center.
Your router has to know where it is in relation to the piece of material you are carving. If you have your origin point in the center in fusion, it would be more forgiving than starting from an edge (corner) if your work piece is not the same dimension as your fusion model. You would also have to invert the second side to have it match the first carve. I hope this helps.

Cheers,
Neil

1 Like

Stradibarrius,
I do a lot of two sided carving on mandolin plates and necks… my experience is that you must have a way to index the piece. For example I build the mandolin top/back in Fusion 360 with index holes in the edge of the stock (clear of the actual part) for .25" wooden dowels that go down into the spoil board. When I turn the board over, the pins fit into the same holes and the machine knows “exactly” where the piece is located… If done right, there is no need to re-zero the machine unless you change bits or move your z-axis reference for the next carve. I will zero the x and y position when I turn the machine on and not change it again during a two sided carve because I design in these index holes that allow me to turn the piece over and use the same zero point. I hope this make sense… on a violin neck, I would put an index hole at each end of your stock. Let me know if I have confused you… I will take some pictures to help explain if necessary. Good Luck.

2 Likes

Vectric also has a video showing what @BillG is explaining. I have used the three hole random pattern method many times to do two sided carves and it is very accurate.

I have also used the three pin method to do multi-color epoxy inlays when I need to take it off the table in between carves.

1 Like

Yes that does help me understand. Thank you for your input! If you have any other ideas I would like to hear those ideas too.

1 Like

You might check out this “Two Cherries Instruments” video on youtube

He is carving a violin neck on a cnc… I’ll say one thing about it though… I have never
seen him use index holes like I use them. He is big on using the “tape down” method and using a fixed rail to index the part. Its hard to argue with his success. The fixed rail part is fine, but I use index holes and clamps with t-tracks to more firmly hold the part in place. I have tried the tape method and now only use it for cuts where accuracy is not critical. If I am trying to, for example carve a mandolin top (double sided) where I want to control the thickness to <.010, I use t-track clamps on all corners and in the middle of each side… tape didnt work in that situation for me. Just some food for thought.

One good thing to take away from his videos in general is that he uses the pocket clearing and then scallop tool paths in Fusion 360… that works well. I usually use parallel tool paths at multiple depths for roughing the part in, but I believe I am going to switch over to his method. I believe it is faster. Parallel toolpaths at multiple depths spend a lot of time cutting air… live and learn!

2 Likes