Compensating for Material Thickness Variations
MDF seems to vary from sheet to sheet as well - same bundle, sheet to sheet. One will leave a slight skin on the bottom, and the next will through cut slightly into the spoil board. I could touch off the spoilboard for the through cuts and retoolpath everything. I really don't want to do that. It would be hours of toolpathing for the number of programs I use. It seems there has to be a better way.
From contributor B:
I think a lock dado is the best way to deal with material thickness differences. If you make your dados 5/8" and run a pass down the tenon to skinny the tenon down to 5/8", then the parts will fit regardless of material thickness. This requires a bit of extra programming work, however.
Is the problem that the parts don't fit in the dados, or that you are not through cutting consistently? I don't understand why you would get a different depth of cut from one sheet to the next. Are you calipering and changing cut depth for each sheet?
From the original questioner:
To contributor B: The lock dado is a heck of an idea.
ďIs the problem that the parts don't fit in the dados, or that you are not through cutting consistently?Ē
It's both problems. Letís say I'm cutting parts out of .5 MDF. I toolpath the part with a cutting depth of .505 inches. I cut one sheet and the parts come out fine with just a slight imprint of the toolpath on the spoilboard. I load the next sheet and cut the same program, the same way. Now this time the parts have a paper thin skin left. Now I have to cut the parts out of the sheet.
As far as the dados, letís say I am cutting out a bookcase and need the center shelf to be fixed. I want to dado the shelf for support. I pull a sheet of ply off the shelf. I want the material to fit the dado correctly but when I measure the material. Letís say it measures at .7253 in. on the edge and I cut the dado at .726 inch - the parts cut from the center of the sheet are thicker than the .726 inch. Now the dados are just slightly too thin to fit the material.
To fix this, I currently have to adjust on the table saw to get it to fit. It seems there should be a way to account for this. I just don't know what it is. But I do like your lock dado idea. I'll re-toolpath everything if I have to and touch off the spoilboard.
From contributor C:
Use a mortise and tenon blind dado. This way you mic at the spoilboard and cut the tenon the same thickness each time. 3/8 from the spoilboard is always 3/8 from the spoilboard. Then you can cut your mortise the same size (3/8 + a smidge) every time. The tenon need not be as long as the width of the part either. In fact you can make it asymmetrical so you know which will be the front and back. Does this make sense?
I also meant to say that you can also purchase material that is sold as exact thickness. (I forget the term for it.) It's a bit more expensive, but that would solve a lot of your problem.
From contributor D:
You said: ďLetís say I'm cutting parts out of .5 MDF. I toolpath the part with a cutting depth of .505 inches. I cut one sheet and the parts come out fine, with just a slight imprint of the toolpath on the spoilboard. I load the next sheet and cut the same program, the same way. Now this time the parts have a paper thin skin left. Now I have to cut the parts out of the sheet.Ē
This sounds like you are having a problem with your Z encoder and it is not hitting its depth consistently each time. If it were working properly it should not matter how much variance in thickness you find in one sheet or a whole bunk and the type of material won't matter either. The top of your spoil board does not change (unless you do a fresh flycut). If your spoilboard is moving you have other problems to work out, but I would first investigate your Z-control.
From the original questioner:
To contributor D: I have always touched off the material, not the spoilboard. I'm starting to see that is the wrong thing to do. It might be something wrong with the Z axis but I bet it's because from sheet to sheet I touch off the material, not the spoilboard.
From contributor E:
Do you touch off on every sheet? If not, and your depth is varying, then you have a machine problem holding depth in Z axis. I prefer to program from the top of my stock but I have developed a pattern of touching off of the spoilboard and then adjusting the z offset the thickness of the material less .005 so it will still cut through. This also allows me to quickly adjust for different material thicknesses quickly by changing my wear offset in z to whatever my material thickness is.
From the original questioner:
To contributor E: I used to touch off every sheet. By doing this the material seemed to have thickness variations - sheet to sheet and edge to middle. Again, this is not consistent. I can mill 10 sheets in a row and they seem to be exactly the same. The 11th sheet, (when touching off the surface of each sheet) would not through cut. Then the 12th sheet (again when touching off each sheet) would cut fine.
I always use air to blow off the touchpad and the material surface before touching off. Lately, I've been touching off in the material surface and cutting. If the sheet gets through cut like I think it should I do not rezero and just keep loading and unleading the machine. This seems to work better. However, I feel this is a band-aid solution. Could it be that maybe the touchpad or has a layer of dust that elevates the pad? This would give an artificial high thickness for the material so maybe that's it? Maybe?
What about the material thickness differences from edge to center? I have verified the change using a digital caliper. Seems if I had a caliper with a 24 inch reach the problem would be solved. Also, I'm in Florida in a non-air-conditioned shop. Could the humidity moving in and out of the edge of the material change the thickness enough to cause this? Supplier has an ambient air warehouse. Thanks for all the suggestions.
From contributor D:
My recommendation is to touch off the top of your spoilboard and let the variance float to the top side of the sheet being machined. The variance should not be so great as to cause any major problems. The only place where you might have to re-think your programs is where you have routed pockets, dados and rabbets, because they can be affected by depth of cut where a tight tolerance is critical. If it's mostly drilling you are doing a hair more or less depth usually doesn't matter.
From contributor F:
This is what I do Ė first, issue depth of cut. I wrote a small pocket program z-.25. I set my tool to top of part then run the pocket program somewhere on the sheet that is not being used, measure depth with a caliper then adjust tool depth on my tool offset page. Next issue width of dado, I measure the thickness of all my sheets adjust the dado to the thickest sheet and cut.
From contributor G:
Everyone has fine suggestions but I am in Ohio and humidity does play a factor in material thickness. When we first got our machine we were very worried about material thickness, but learned very quickly that we had to find a happy medium ground. Also spend the extra money on good board; it is well worth it in the long run. After banging my head trying to make everything perfect I remember something an old Engineer told me KISS = keep it simple stupid. I quickly realized we were over engineering. The moral to the story is to keep it as simple as possible and find a happy medium. It will help you very much in the long run. A CNC wood product is not an exact science so you have to figure out what tolerance you can live with.
From contributor H:
In the past I have had three p2p's and depth was always an issue. When we got a fourth KOMO router and we touched off to the machine zero (the MDF table). This established z zero every time the problems seemed to go away. As for the p2p and using the machine data in the controller to modify your tooling, this still proved to be hit or miss. The pods may be out or you have an after market pod in the mix and one corner of the part is high or low and the dado is effect. The CNC works off of machine Z zero and not the top of the part. The CNC can guarantee what is remaining of the panel and not the depth of every groove or dado.
Are all of your parts dadoed or are some cross rail just doweled? This was always a problem. You could take a sample of say 25 or 50 sheets and come up with a range and average thickness of a sheet. At one point we were machining 250 sheets of Baltic Birch a day. You talk about a thickness problem!!! Many of the cabinets were dado construction and we found a dado with that worked. 15mm BBB Baltic Birch measured anywhere from 14.1mm to 15.7mm we used 14.7mm because the range was on the higher side although the average was lower. QC at our plant just had to live with it - after all we make cabinets and not rockets. At that volume you canít adjust for each sheet or part. This is the fun part of what we do.
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?