Panel Positioning for Machining on Both Faces

Advice on maintaining precision when machining both faces of panel stock on a CNC router. April 17, 2009

We have a product line which has machining on both sides of parts. How do I set this up on a flat table machine? I have pins in one corner. I need this to be nested on a 4' x 8' sheet. Any suggestions on techniques would be much appreciated. Machine is an AXYZ 4008.

Forum Responses
(CNC Forum)
From contributor M:
My normal method is to cut the most complex sides in the nest and cut the perimeters, then turn over the parts that need machining on the back and cut them at the pins.

You need to keep track of orientation; it's easy to put a part for secondary ops on the router in the wrong orientation, and I normally label the part in such a way to make this easy. For example, adopt a convention that your label goes in the corner of a part that then goes to the pins.

Also, be sure your machine is correctly calibrated for a home position right at the pins. Some people, who always nest, gloss over the fine positioning at the corner of the machine, or offset this positioning to allow for trim. It isn't hard to calibrate most machines accurately and well worth the small effort.

Another strategy is to trim side A on the machine to a perfect perimeter slightly smaller than your nominal sheet size and do the operations required for the backs all in one step, then turn the whole sheet over and machine the fronts and cut the perimeters.

I don't prefer this myself for cabinet parts. Secondary operations are usually not done on a whole lot of parts and I find it too difficult and labor intensive to program this way. You mentioned a product line though, and if you have a lot of repeats of sheets that you run over and over again, doing the secondary ops on a full sheet, then flipping the sheet to do primary ops and cut perimeters will work well and reduce load/unload time.

From contributor J:
AlphaCAM has a reverse side nesting feature that will do this.

From contributor R:
More depends on your software than your machine. As stated above, there should be a second home position to relate to for the second operation. Some machines can be difficult to locate smaller parts. A Thermwood I work with has widely spaced pins. Fine for sheets, but way too far apart for a cabinet side or such.

A fairly simple jig can be made to latch to the side of the table to properly orient the part. Use the machine to mill the locating faces relative to the proper home (once the jig is in place) and it will be dead accurate.

From the original questioner:
The panels I'm starting with range from 80-96" in length and 33-11" in width. Material will be 3/8" MDF. There are grooves on the back and front. Each panel is symmetrical along the center of the panel.

I like the idea regarding the squaring of the perimeter, which will give me a square and accurate edge for secondary operations and alignment.

I do my design in AutoCAD, then set up the machining parameters in Toolpath software, which came with the AXYZ machine.

From contributor L:
We do the same as contributor M. Our machine has two fixed pins and one that slides in a machined groove in the edge of the table. That allows any size part to be referenced.

From contributor W:
Yes, I agree - you should cut the piece square before flipping it to get the best accuracy. What you could do is assign each side that needs machining to separate groups in your ToolPATH software. This way you could just turn off one of the groups and send the file to the machine for side one, and then turn on the other group and off on the first one and send the second file to the machine.

From contributor K:
Router-CIM has fully automatic 2 sided nesting in their advanced nesting module. Komo was cutting 2 sided nested sheets at IWF this year.

The software cuts the back side of the sheet first, then does a trim cut along the edge and side of the sheet so that there is a machined edge to flip the sheet over and position very accurately against the pins. The front of the sheet is then cut. Another option is to cut half way through on the back, flip the sheet and cut the other half way through on the front.
You can get bull nose parts without elevating the sheet. You also don't need to resurface the spoil board using this method, saving time and money.

From the original questioner:
Thanks, but I don't need more software. Just looking for the technique. I did the trim cut to square my sheet and the parts came out just right and within specs. Will a thinner spoil board be better or worse for vacuum hold down?

From contributor J:
I've not seen any evidence that the thickness of the spoilboard improves or decreases part hold down. In other words, anything from .75" and thinner will work. One word of caution: if you're drilling through holes, a thin spoilboard can allow the drill to penetrate into the table of the machine.

The primary factors are:
1. Cleaning and maintaining the filters in the pump.

2. Cleaning and maintaining the vacuum seal under the spoilboard.

3. The right size and type of pump.

4. Surfacing both sides of the spoilboard. A spoilboard with through cuts will leak through the cuts, under the parts.

5. Size of the parts - some small parts require onion skinning and/or tabbing.

6. The right type of spoilboard. The vast majority of operators use regular MDF. A few report better performance with lightweight MDF. In my opinion, lightweight MDF is too porous, pulling too much air through the edges and through any uncovered portions of the face.

7. Condition of the spoilboard: damage to the edge of the spoilboard can cause excess airflow through the edge.

8. Open area on the spoilboard. Match the size of your spoilboard to the material you're cutting and gasket under the spoilboard. If the part to be cut is smaller than the spoilboard, cover the open areas of the spoilboard with 1/4" melamine or other non-porous material.

From contributor R:
That is a great idea. Cutting the flip operations first totally solves the part locating issue, especially for machines like I mentioned above where the locator pins are set too far apart for smaller parts.

To the original questioner: This idea may well work for your application. It should be fairly easy in CAD to lay out the flip operations on the back of the full sheet. Give it some thought.

From contributor W:
AXYZ Toolpath software is about the easiest software I've ever used. Just some better thinking of your layout in CAD is all that's needed. KOMO and AXYZ are about as far apart as you can go on the CNC scale and I would be impressed if Router-CIM had a post to be able to import that into the Toolpath software, as the only link to the machine is to go through the Toolpath software.

I ran an AXYZ machine for 6 years at a sign shop and a few times I had to do two sided work, since I only had clamps and no vacuum. I secured a piece of 1" MDF to the bed, then ran my file for one side and also routed four to six 1/2" holes through the material and halfway into the 1" MDF. I then flipped the sheet and inserted 1/2" steel dowels to locate the sheet after flipping to run the next file.