part to long for machine (Newb question)

I just watched a video of a guy working on a part that was to long for the machine.
Looks like he used V-Carve Pro to do this. "Tiling" is what he called it.
Is there another way to do this without using V-Carve pro?
Thanks
OSD

You'll have to be more specific about what you're trying to do and what the configuration of your machine is. For example, I used to have a machine that had a 4'x8' bed which was open on three sides, so I could slide material either direction and continue cutting a contiguous piece of material, or I could rotate it and cut an adjacent section of a panel that is too wide (like a 5'x5' baltic birch panel). Now I have a 4x4 machine with a stationary gantry, so I can't cut anything wider than 4' in one direction, such as the baltic birch panels, but I can cut parts longer than the 8 ft. The machine configurations can be more or less limiting if you are planning to work in a single piece of stock.

If the part is to be cut from a contiguous piece of material, you need to locate the material for the second cut. This can be done very precisely by drilling indexing holes for pins to relocate the part on the table in a new location. If you translate the holes in the CAD drawing with the part as it gets moved on the work table, you can use those translated holes to relocate the part and the second cut should match up very well (usually within a few thousandths of an inch. If you don't need high precision, and you have a work table that you can cut into a bit (wasteboard), shift some of the first cut geometry over in CAD, then cut it into the table so you can line up the edges of what you've already cut with the new location. This can still be very accurate with experience and careful placement, but isn't completely fool proof either. I would guess that I can usually keep the part placed within .010" by sight if there is enough overlap between cuts to make it clear how it should sit.

Hope that helps, but if you want more you'll need to let us know what software you plan to use, what your machine is configured like and what kind of tolerances you hope to maintain. Even an example of a part would make it easier to show how it could be done in a simulation. Otherwise, the answer about V-Carve is "No", you don't need to use V-Carve to "tile" or index your cuts to produce oversized parts.

Here's a quick video showing a method to index parts:

https://www.youtube.com/watch?v=Hhdu...ature=youtu.be

Thanks for responding mmoe!
My machine is a DIY cnc router ,X is 44", while Y is 30", so I would use the long piece on the Y axis. At this moment I'm using Solid Works (student version) with HSMexpress for cam to Mach3. However I'm going to use Freecad with Heekscam when the student version runs out.
So I added a file that has a continuous piece of 3/4" plywood and I added a reference hole.
I don't know how to transfer geometry, I'm a Newb so I need a lot of hand holding!
Thanks again
OSD

Just saw your post for youtube! Must have sent my post just a second later!
Thanks for the reply!
I'll have to experiment.
Thanks
OSD

I went to bed thinking about how to do this. Couldn't come up up a solution of how to divide the part into segments. I don't know if this is a CAD or CAM problem. Any suggestion?

There are really several ways you could do it, but I can only show you the way that I would do it with the software that I use personally. It may or may not be helpful to you since I can't say that you'll have the same functionality. My tools of choice are Viacad 2d/3d which runs about $35-$90 depending on which release (or Pro if you want to spend more). Version 8 is as good as you really need, and runs $35, but you can spend $100 and go with the most recent release. While it rund $35 more than Freecad, I don't think it's $35 you'd regret spending. I have other software such as Rhino and Bonzai 3d, which cost a lot more, but I still use Viacad for the majority of my work which I think says a lot about how well it works. It's occasionally a bit buggy, but so much more efficient that I don't mind putting up with the minor quirkiness (which is pretty minor in my experience).

I also use Bobcad/cam for the CAM portion of my work. I currently use V26, which has been nothing short of excellent overall. Again, it's not a free program, but with that comes more expectations and functionality. I don't want to say what you could probably buy it for, other than to say their list prices are not very close to what the average Joe pays for it. In the past, Bobcad was OK on features and apparently annoying about salesmanship, but I've had it for over a decade and have never had anything but positive experiences with them and their product. Either way, the easiest approach to cutting these parts would be simply to locate where you want each section to reference from and then use the "Machine Setup" feature of Bobcad, which allows you to create a new origin relative to the geometry without even moving the geometry. Basically, you pick where you want "0,0,0" to be for each program (one program required for each section machined. You also would need to cut the geometry into segments that allow it to be used to produce code that overlaps. I've already discarded the first example, so I'll do the same thing on a fresh drawing showing how I did it at the CAD side and the CAM side. You could do the same thing using other methods, but I'll show what I think is probably the easiest. Whether or not the same functions are in the software you use, I can't say, so you may have to adapt to what you can do with what you have. I'll put a quick video together and post it up in a bit.

Thanks
OSD

This is kind of a hard operation to show in a video as I'm trying to do it, mostly because there are some time limits in how long I have to produce the video without having to get pretty serious about doing some video editing. Plus, the video capture software really slows down the whole system a ton, so it's hard to use the software efficiently while capturing video (makes it very choppy). With that in mind, I skipped showing me actually draw the file I generate code from, but I've attached it as a DWG file so you can look at it. I did not show programming the first step, which is to drill the holes in the table wasteboard surface to use for indexing the second cut. You drill those holes without stock in the way, then install the stock and cut the part as well as drilling holes in the stock that allow you to shift the part to align with the holes in the table for the second cut. If you can do it with origins as I do in Bobcad, you only need to draw the entire shape and the indexing pin holes located at the correct distance apart for this to work, but you'll see in the simulation that the sheet is still shifted even though I don't have to shift the geometry. This is a very nice feature of Bobcad. Using these holes as the reference origin for each step of machining will pretty much ensure that the alignment is good. You'll notice that I was particular about being sure the second origin point was properly located with the center snap of the circle (sometimes it catches the center better if I zoom out before selecting the circle). You'll also notice that the simulation shows that the parts are virtually perfectly aligned, so the origins were obviously snapped well. If I see something wrong at the simulation, that's often the issue (that the origins are off).

If you don't have that capability in your CAM software, you need to draw two different CAD files and program them independently, again based off of the indexing pin holes as reference origins. It works the same, but is a little more time consuming since you'd have to essentially make two separate files and manually shift the part in the second file to align with the first file. In order to get the second cut aligned to the first cut, you just move the part in CAD so that the pin holes you drill in the first op are perfectly aligned to the pin holes you drilled in the table before you started cutting the stock. This is the same concept as moving the origin in Bobcad, but instead of moving the origin, you're moving the part in relation to the same origin you used in the first op. Hope that makes sense.

Download for video (about 26mb):
https://files.secureserver.net/0s1kYqCoGb00Xx

Also, the changing of the work offset I do in the video only affects the simulation. If I send code out from the machine, it's the same no matter what the work offset is configured to be. This is why the part is hovering over the table the first time I simulate, but then it moves down to the table surface the second time. At the actual machine, machine zero is up at the top of the Z axis stroke and just beyond the edges of my table in X and Y, so I have to zero the cutter to the top of the stock, then adjust the zero position for X and Y to somewhere within the table surface. In Bobcad, I have to do the same thing using the work offset just as you would in Mach 3 when setting up the G54 work offset for cutting a part. Really, the simulation machine works in nearly identical fashion to the real machine, and the real machine also requires those offsets be entered.