First id like to apologize if this has already been answered, i could not find a thread that covered my issue specifically.
im currently machining a bunch of duplicate small parts nested on both sides and im having an issue where the reverse side is offset by about 2mm each time. im at wits end. ive gone over and over and over with the models and tool paths in fusion and ive even torn apart my entire machine and enclosure, tracked and made sure the machine was a perfect square using this video https://youtu.be/lU0iZKajpoo?si=EdZVuSTePfgxG67W
and im still having the same problem i began with. still about 2mm off to the left.
im using:
woodworker
fusion 360
3 pin method with hardened steel pins
From your description are you setting up something like this:
If so then be aware that the width of your part becomes extremely critical when you are using the front left corner for both sides.
If you are off by 1mm on the width compared to what your software expects then the other side of the carve will be off by 2mm.
In this case use the front right corner for the 2nd side origin.
I forgot to clarify that I was thinking of origins in F360. One method that can avoid the potential error pointed out by Chris is to use a pin centre as the origin and machine the receptacle for the pins (2 required) on the first side. Then when flipped over it always locates the other side correctly for machining. I do this all the time for loudspeaker baffles for example.
@wood
Am a rank tyro here compared to the big boys but,
I use two hold down bolts on the work, outside of the carve. the bolts thread into the t nuts under my spoilboard, I locate the center of the piece between the bolts, ( I use nylon bolts if I am worried about the bit hitting them & since I cut it close i have hit a couple of bolts) Easel ( the kiddies software) lets me center the cut & by using the bolts, I can flip the work once a side is done & get very close in both X and Y axis. This method does not rely on exact sizing of the blank as it centers on the hold down bolts. Once I have set the offsets at X0 Y0 all I have to do is probe the height for each carve. Dead simple and very quick if you keep a ratchet handy. Far faster than any other method I have used. If you do not have t nuts under your spoil board you can easily make a small spoil board with appropriate fastenings for the hold down bolts.
No tape and glue, no clamps or cam wedges. I can either calculate the center by locating the X & Y for the nuts, or I made to short studs with points on the top thread them in and position the work on top & give it a tap with a soft hammer then drill the indents on the drill press, you could cut them in with the CNC but the drill press is quicker. If doing a high volume a fixture for the DP would be easy.
Hope this helps, Just started using it a week or two ago and just love it.
That is a nice looking carve you are doing.
Aside from where you set your X and Y zero point as mentioned previously, I’d like to bring more attention to the two schools of thought regarding registration hole placement.
I also wanted to claim outright, that although I have done many two-sided projects, I am by no means an expert and barely know the finer details of this process as hopefully other more seasoned machinists may provide.
The first method of flipping revolves around (pun intended) placing the holes in an asymmetric, or random, pattern. With this method, there is only a single way the second side will align to the holes. And, the registration holes will only work for the second side. Once the first side is removed from the clamps, you can’t really flip the workpiece over and go back to it for additional carvings. You also have to be careful how you drill the holes in the spoilboard for this method. Particularly, you have to make sure the spoilboard holes are flipped according to the direction you planned on flipping the workpiece, that being horizontal or vertical. If you don’t flip them in software, they may appear lined up, but can be off by a few millimeters.
The second method is where you evenly space all the holes based on the 0/0 origin point, or a common reference like the center or edges of a vector. This method doesn’t require flipping any of the vectors like the asymmetric method, but alignment of the holes in software needs to be spot on, otherwise it may introduce alignment errors.
I personally have settled on using the symmetric, or evenly spaced, holes, and usually drill 4 of them; one in each corner. I chose this because I many times will perform a surfacing operation on the top side in lieu of a jointer or planer. With a perfectly flat side, that is also perfectly parallel to my spindle, I then flip the piece over to not only surface the bottom side, but then carve things like my signature, dates, keyhole slot, etc. This means I have to flip the piece once more (back to the top) to finish the carving. Also, my OCD dictates things like this are spaced evenly.
@SurfinGump
I have tnuts spaced at 40mm long both the X & Y axis, so I just decide which two to use and drill appropriate holes in the blank, it is not much work to plot the center of any pair. I drill the blank for a close fit, and I find this to be accurate enough for my work usually am within 0.5mm, if I start finding that this is not close enough can easily make a few adjustments like using flat head machine screws so the tapered head tends to pull the work inline. One solution never works for everyone or everytime but just thought I would describe my way. As mentioned am by no means expert cnc’er but have many years woodworking and manufacturing experience in several fields.
So let me explain in a bit more detail, what I’m doing.
i have a jig that’s essentially a machined flat sacrificial piece that has bolt holes located to fit my spoil board.
I then take my material and double sided tape it to the “jig” and machine 3 holes two on the sides and one on top.
next I press in my steel pins (I’m not worried about striking them).
then I machine the front, then turn the material over and machine the back.
the back side is exactly the same as the front, same tool path file and everything.
so the piece is located via pins through the material, the file for front and back are the same, yet the back side is always about 2mm off to the left?
I’m going to re-read everyone’s responses, as I’m still a newbie and may just not be completely comprehending what’s being presented to me, but I thought I’d add more information.
Is there perfect symmetry left and right for the parts and for their locations through the vertical axis intersecting the centre pin? And is your datum for each side in F360 coincident with this axis of symmetry?
@SurfinGump
I find that two bolts is sufficient, but of course four bolts would be a little more accurate, the only adjustment you (and I) need to make is to probe for Z,
When you are creating the machining Setup in Fusion 360, are you using the “Extra Stock”? I’m traveling so I might have the wrong term. But it will assign an extra 1mm to sides and top for machining away. If you then zero on a corner of the stock, the machining object will be 1mm inward.
I don’t do the pin method. I make my wood slightly oversized and then use a 1/2" end mill to cut it to the correct dimensions. That way all I need to do is get the edge closest to the front parallel to the X axis. When I flip the project I use the touch plate to set the new zero.
When I surfaced my spoilboard the bit didn’t surface all the way to the front edge. It left a lip that’s parallel. That lip acts like using pins to get the project correctly positioned.
