Common Line/Chain Cut Nesting and Toolpathing help

[ArtisanzKA]

Hi there,

I recently got a CNC router and it is something new to me. I have a lot of experience with ProNest and cutting in the 2D realm with a CNC plasma and waterjet. I know in ProNest how to do what is called "chain cutting" where the head does not stop cutting between discrete parts and continues on a path as well as common line cutting.

I am going to include pictures that show the tooling I have to do this job as well as a finished part that we subbed out to someone to cut for us in the past. I'll do my best to describe what I'm thinking I need to do.

First what I already am familiar with in the software - I have used it to cut out a nest of parts on a sheet that used one tool, but I do see how I can use the software to do tool changes depending on the toolpath specified. I just want to make sure you guys don't waste your time going over information I already know. So I'm not completely starting from scratch

Now the part -




The material is 1" thick HDPE. I plan on cutting all of the "windows" out of the center of each part in the nest first with the quarter inch endmill bit


Now is where I am needing help on the second operation with the 1/2" endmill bit.... I want to start from outside of my material and create a path into the first part and cut the entire outside profile and WITHOUT LEAVING THE SHEET continue onto the next part, essentially continuing in a chain around each successive part until I get to the last part. I plan on coming down .875"-.9375" into my 1" material leaving material on the bottom to keep the parts in place for my third operation. This process will create a 1/2" channel around each part now as well as a small amount of material at the bottom to keep things in place. I will need this toolpath to also lead a channel OUT of the sheet for my third operation tool...


Now this tool I want to essentially use the same path as the 2nd operation and leave a radius edge on top and bottom of my parts.

Is any of this possible or feasible? Any advice would greatly be appreciated. I am being expected to figure all of this out despite 0 experience running a CNC router or really any tooling of any sort....

Thanks everyone. The person that sold me the machinery highly recommended this forum for help on what I needed to do. He had no advice to offer me on this particular job. As this is my first post if I have breached any etiquette I am truly sorry I'm just in a scramble to try and solve this conundrum.

[Adrian]

I'm not following what you mean by "not leaving the sheet". Do you want to cut straight to the next part without the bit retracting? I can't see why you would want to do that but I can't think what else you would mean.

[ArtisanzKA]

I'm not following what you mean by "not leaving the sheet". Do you want to cut straight to the next part without the bit retracting? I can't see why you would want to do that but I can't think what else you would mean.

Correct. It's called chain cutting or chain nesting. I do it on my plasma from time to time.

But I need to chain these parts together for a contiguous cutting path because I don't want to plunge with the profile bit.

Edit- Also as I said in the original post, I need to start the toolpath from outside the material initially and end the program outside.

[Adrian]

I wasn't following what you meant to start with as you mentioned the chain cutting starting with the 1/2" bit. I see what you mean now as you would need to cut a trench with the 1/2" bit for the profile bit.

Basically the only way you're going to do it is to edit the g-code to remove the z-retracts, draw the design as one continuous vector or create lead-in, lead-out vectors to the edge of the sheet (or maybe get creative with the built-in leads function).

Basically there's no push button solution for multiple parts like that.

[Rcnewcomb]

I've only seen that feature in CAM software that is in the $4K-$40K per seat price range. With Vectric products you would need to determine the chaining path yourself. If this is a one-off job, or if it is exactly the same job over and over then it might not be too bad to figure out. If you have a lot of this type of work coming your way with many variations then you may want to consider a more expensive software solution.

[tomgardiner]

Aside from the chain cutting I foresee difficulty holding the parts in place while running your final pass. There isn't much surfaces area for the vacuum to hold.
Is the minor diameter of the rounding bit 1/2"? Otherwise you will have to offset the initial 1/2" EM cut to compensate
My limited understanding of plasma cutting makes me think that there is more of an issue starting cuts and hence the rationale for chain cutting. It is less problematic to lift and start a cut particularly in HDPE which cuts like butter.
Part holding though I think will be your biggest issue.

[TReischl]

Chain cutting is done because on certain machines, hi speed plasmas and lasers it is faster to just keep cutting to the next part rather than turn the beam move pierce and start cutting. It is entirely possible that it would be a bit faster on a router too. Or maybe not. My hunch here is that all the fooling around setting up to make that cut will eat up way more time programming.

And yea, I know, a programmer can be working while the machine is cutting. But the programmer has to be paid for too. An often overlooked concept.

[ArtisanzKA]

Chain cutting is done because on certain machines, hi speed plasmas and lasers it is faster to just keep cutting to the next part rather than turn the beam move pierce and start cutting. It is entirely possible that it would be a bit faster on a router too. Or maybe not. My hunch here is that all the fooling around setting up to make that cut will eat up way more time programming.

And yea, I know, a programmer can be working while the machine is cutting. But the programmer has to be paid for too. An often overlooked concept.

I have to do everything. Engineering, programming, operation. And of course everything has to happen tomorrow.

Dunno what I'm going to do at this point.

[tomgardiner]

How many of these are you making? Here is what I would do.
I would rout all the profiles with one bit. I assume that you are using a 1/4" bit to maintain a small radius corner so run it two passes leaving ± .010 " onion skin (adjust for flatness of sheet)
Next I would use a single sided plunge round over to profile the top edges. Cut the parts from the sheet with a knife. Clean up the internal edge with a deburring tool and round the exterior on a router table (all done while the next sheet is running)
It ain't elegant but it will be quick and reliable.

[ArtisanzKA]

How many of these are you making? Here is what I would do.
I would rout all the profiles with one bit. I assume that you are using a 1/4" bit to maintain a small radius corner so run it two passes leaving ± .010 " onion skin (adjust for flatness of sheet)
Next I would use a single sided plunge round over to profile the top edges. Cut the parts from the sheet with a knife. Clean up the internal edge with a deburring tool and round the exterior on a router table (all done while the next sheet is running)
It ain't elegant but it will be quick and reliable.

I have literally thousands to do , but thanks for the suggestion. I'm thinking of routing out the 2d profile and building a jig that uses the central window section of the part as a hold and putting the radius profile bit on a mill and finishing them that way.

[tomgardiner]

Okay how about this? Cut out all the internal pieces and cut the outside profile leaving a generous onion skin of 1/16" or more. Round over the top edges. Cut all your sheets for the production run.
Now make a fixture to register and hold the parts in place by milling a sheet of ply leaving raised sections equal to the internal openings (mirrored). Flip your sheet onto the fixture and tap down. Run the roundover for the back side.
This may be too finicky to get the sheet to drop onto the fixture without fighting with it. If so break the sheet up into only a few rows of pieces still held together.
I did a similar job in HDPE with hundreds of vents that had to be milled on two sides. I ended up cutting the parts out fully then machining a 4 x 8 fixture with recesses to hold each piece for chamfering. It was slow to load but the savings were in not having to hand chamfer.

[ArtisanzKA]

Okay how about this? Cut out all the internal pieces and cut the outside profile leaving a generous onion skin of 1/16" or more. Round over the top edges. Cut all your sheets for the production run.
Now make a fixture to register and hold the parts in place by milling a sheet of ply leaving raised sections equal to the internal openings (mirrored). Flip your sheet onto the fixture and tap down. Run the roundover for the back side.
This may be too finicky to get the sheet to drop onto the fixture without fighting with it. If so break the sheet up into only a few rows of pieces still held together.
I did a similar job in HDPE with hundreds of vents that had to be milled on two sides. I ended up cutting the parts out fully then machining a 4 x 8 fixture with recesses to hold each piece for chamfering. It was slow to load but the savings were in not having to hand chamfer.

Now we're talking.... That isn't a bad idea at all. I think I could probably make that work.

Thank you!