|Home » Forums » CNC » Message||Login|
You are not logged in. Consider these WOODWEB Member advantages:
Design for CNC - tips for 18mm Baltic Birch5/9
I'm designing some furniture that will be cut on an CNC machine out of 18mm Baltic birch plywood. After I get a pre-production prototype I'm happy with I plan to kickstart it with a minimum initial batch of 50.
Question 1: Will I need to chamfer or otherwise relieve the edges of the holes in case the glue swells the grain around the hole?
Question 2: How accurate can I expect things to be on the Z axis? I thought +/- .010” was reasonable… but this shop was way off. It worked for the prototype, but it wouldn’t work on production runs. Am I asking too much of CNC? I don’t think they had a vacuum hold down system.
Question 3: Due to the number of holes (3 different sizes), I know I will need to send this to a shop with a tool changer. Should I strive to make sure the majority of the non-hole features can be cut by a 3/8” bit instead of a 1/4” bit?
Question 4: I’m plan to do my own nesting, primarily to make sure I can keep my materials cost down. If I am cutting two parts next to each other, I assume I should keep the parts farther than one tool diameter apart so you don’t cut both edges (one climb, one conventional cut) at the same time? So that both parts can be cut climb or conventional as fits the bit / material?
Question 5: Any face to face joining techniques I should look at other than dowel pins? I am worried about glue squeeze out.
Question 6: Other than making parts self-align and making it easy to assemble by keeping part count and confusion down, what else can I do to make this cheaper and easier to manufacture? I’m planning on a clear polyurethane finish.
Thanks for any help you can give!
My thoughts are:
All the parts will be cut "good side down" and then get glued together to show the good sides on the outside.
90% of what we cut is baltic birch.
Any design that needs a tolerance of 0.010 Z using wood needs a rethink - too many factors involved.
The quickest way to the best finish is a 1/2 compression spiral chipbreaker as a 0.020 oversize first pass and a 1/2 downspiral finish pass. We run the first at 750 or 800 IPM and the finish (if needed) at 500 to 600.
I leave 13mm between parts on a nest.
You don't mention the size of your parts, but we do many small parts. We cut these 16.5mm deep and then separate on a trim router. We use an upspiral flush trim bit for best edge finish.
Nesting yourself sounds like a good idea, but if the shop you deal with has decent nesting software don't waste your time. They can do it better and quicker than you can.
Hourly rate is a bad way to have people quote. I charge $140.00 per hour and am usually lowest cost per part when compared to people in the $100.00 per hour range.
Where I am 5X5 BB is less cost per square foot than 4X8 so look for 5X10 table. Load/unload and tool change time divided by 50 square feet instead of 32. Over time it's a big deal.
If you are using full sheets it might be more efficient to use vacuum bagging to bond them together unless you have a press.All you need is a plastic sheet and a flat surface.A piece of breather cloth is handy too and the stack can be as many sheets as you like.Even clamping pressure and much greater force to minimise the glue line thickness and glue usage.You can use masking tape to align the edges or 2 small pins per sheet.I have found online nesting available for rectangular shapes and you set the parameters to match your needs.
Only thing I can contribute to what others have said is to consider gluing your sheet goods together before the cnc. We do this on a regular basis, just apply glue to both pieces, align them and place them in the press. CNC time will be slightly decreased over-all due to only handling half the number of parts, even though the actual spindle run time may be exactly the same. I also find that two pieces glued together seem to stay a little flatter on the vacuum table than a single sheet.