I just cut a job where I added pilot holes for screws via the Part Editor. They were 1/8" diameter through cuts.
When I ran the job the holes were not drilled completely through the material. My shelf pin holes on partitions which are through cuts fell short as well.
The code written for both was correct, the thickness of material plus the cut through depth amount but they still didn't drill through.
Is this a material thickness setting problem? Did these cuts not go through because they are considered pocket cuts and not actual through cuts?
I am just looking for some ideas on what I did wrong.
The pilot holes are going to be great when I get them right. As it was I still had to drill them all by hand.
Kerry, if you look at the 5mm drill bit I would bet the tip is lower than the outside points. Most of the bits I have ever used are this way. You will have to add about .04" in length to the daylight value every time you do a tool length. If you look closely at the parts you can probably see a very small hole where the tip came through. Forrest
I can sure do that with the 1/8" drill for pilot holes but my shelf pin holes are actually 9/32" holes because I use grommets in them. The machine uses the 1/4" compression to interpolate these. I don't want to change daylight on this tool as it also cuts the tenons for the blind dadoes. I may have to add a 1/4" up spiral to drill with when I run my jobs. Or I might un-check drill and interpolate on the 1/4" compression tool and see if the machine would pick up the 5mm to drill the pin holes.
I would still like to know what causes this problem in the first place. Adjusting daylight will do as a workaround but you wouldn't want to do that on a tool used for different operations where tool length is critical.
It is my understanding that the machine knows where the top of the table board is plus the current waste board thickness. When an operation is performed like cutout, the machine references this and adds the amount you have entered as Cut Through Depth and that is cut into the waste board.
Do these part editor holes that are selected to "Cut Through" in the part editor reference the top of the table and waste board or are they pocket cuts referenced from the top of the material being cut?
It seems that when you choose to Cut Through a material the reference should be to the table board/waste board as your material thickness can vary several thousandths of an inch in the same sheet causing problems if these cuts are regarded as pocket cuts and referenced from the top of the material.
Hi Kerry,
To my knowledge, cut through depth does not apply to drilling operations. I believe they ONLY apply to outline operations.
The 5mm tool would be better to interpolate with anyway, and a shallow dado operation will cause tearout if done with the upshear portion of a compression tool. You may not have these other issues, but it sounds like you've already got it figured out already!
jnr
Josh Rayburn
Hall's Edge, Inc.
CNC Machining Service
I'm sorry Kerry I thought you were referring to a brad point bit which always has to be adjusted to get a clean drill through. As far as the interpolated holes for through shelf holes or any edited parts I don't know where your problem is. Everything is working on my end.
Forrest
You gave me good information. Adjusting daylight will work great for the pilot hole drill if I can't discover what I have done wrong.
Right now I am leaning toward using an incorrect material thickness. I measured this in several places (there was quite a variation) and just went with the middle of these. Next time I will go with the thicker measurements. I am also going to get some calipers that will measure away from the edges.
I would still like through cuts, including drilling to use the top of the waste board as their reference point. Then they would always go through.
Kerry, the thickness of the material really has nothing to do with the cut through. If you are drilling or cutting through the machine goes to the waste board with the added cut through. If everything is setup properly you should not be having any issues. Also you are setting yourself up for a lot of frustration if you try to over measure your sheet goods. Take an average and stick with it. There will be some small variations, but overall the finish product will be the same. Forrest
Forrest is right Kerry, adjusting daylight values instead of adjusting sheet thicknesses is the best way to accomplish what you're after. If you need the same tool to do an additional type of operation, set it up in tooling management as another tool pointing to the same toolholder and measure it but don't adjust the daylight. Also add it to tooling setup in CN and set that tool to do the other operation.
For example, set up tool numbers 2 and 3 in tooling management. Both are a 5mm upshear. It is physically the same tool.
Both are setup to point to toolholder 1-3 (position-actuator) or wherever it is.
Setup T2 in CN to do drilling and interpolation. Measure it and add .02" to the daylight value.
Setup T3 in CN to do pocketing or rout / dado or whatever you want, and measure without changing the daylight.
Hope this helps,
jnr
Josh Rayburn
Hall's Edge, Inc.
CNC Machining Service
I believe that what Josh pointed out is your issue. When you specify a ROUND hole to "cut through" in ecabs, CN treats it as a drill, and the "cut through" amount in CN is not added to it. Therefore, instead of cutting to the wasteboard + cut-through as it would do on a straight-line cut, it IS using the material thickness; a through-drill is actually a .75" deep hole, instead of wasteboard + cut-through amount... therefore if the material is .76", you end up not going all the way through.
I have this issue all the time with holes added in the PE, and I'm pretty sure this is how/why it does what it does. Here's something to try: (I have NOT tried this, not sure if it will work!) When you specify the hole in PE, instead of checking "cut through," specify a depth that is .76" if your material is .75" for instance.
The machine can only see that the part is cut through. Any measurement deeper than the material is thick will have no bearing on the machine cutting deeper. If it did you could have real problems with people putting numbers in wrong and your z axis crashing. When adding a part edit with a specific depth like .5" in a .75" material the machine will look at the depth of cut in reference from the surface of the waste board. No matter the thickness of the material the machine is still going to cut down to .25" in Z axis. Unless you change the thickness this will remain at .25" from the bottom of the cut. If you do change the thickness through cuts should still be through period. Forrest
That's true Forrest but it was not always that way....we tattooed some wasteboards very nicely from that oversight in the past... Thank goodness it's fixed now!
Josh Rayburn
Hall's Edge, Inc.
CNC Machining Service
What I am trying to determine is if the machine is looking at these holes created in the part editor as drills or as pockets.
In experimenting we set the cut through up to .003 to see if we could get the holes to come through. My material thickness average was .730. The code for the drilling operations was Z-.733. If my material thickness was actually .740 then the holes would not penetrate as pockets. If the machine is looking for the top of the wasteboard they would penetrate even if the material thickness was actually .750. The same goes for the shelf pin holes. The code writtien for them was Z-.733 and they did not go through either. Are these pocket cuts and not drills?
By the way with the cut through at .003 the other tools were scoring the wasteboard pretty deep
If the hole is round and you have a drill bit the correct size it will drill it. Otherwise it will pocket it. I was not aware that the cut through didn't affect all tools. If your code is correct but you are not getting the desired results something is wrong at the machine. Forrest
