Printable View
This is my first CNC project.
The project is basically to create a flat ring with a thickness of 0.25" with an ID cut and OD cut. The material is fiberglass over balsa.
I have set DeskProto to do a rough cut and a finishing cut with a 1/8" end mill bit.
Does this sound like a good strategy?
Greg
Hi Greg,
The strategy to first do a rough cut and then a finishing cut is OK.
Whether or not the cutter is a good choice depends on the geometry: for curved surfaces a ballnose cutter will be best, and in case of small details a smaller cutter may be needed for finishing.
I am not sure what you mean with "ID cut" and "OD cut": is it Inside Diameter and Outside Diameter ?
In that case you will not be using a fourth axis (rotary axis) for cutting, you will be cutting circles though a flat slab of material.
You then will need to add supports that keep the ring connected to the rest of the material while machining, otherwise is will be loose after roughing.
Hope that this will indeed help you, as I am not sure what the actual question is....
Lex.
Thanks you, Lex, for taking the time to ask your question.
"Yes", for your correct assumption of the meaning ID and OD. I attached a pic of the roughing operation. I added 2 tabs to hold the part during machining.
I am unclear as to what "Rules of Thumb" I should use for the "Distance between toolpaths" and "Stepsize along toolpath". Could you give me some guidance?
Greg
Hi Greg,
It is good that you attached an image, as that shows much more than only words.
As the top surface to be machined (the side of the ring) and the tip of your cutter both are flat you can select a far higher distance between the toolpaths and thus save a lot of time. For instance 0.05"(D/5) instead of the current 0.0076"(D/33).
For the Roughing operation it may even be .083"(D/3). Also enter a thin Skin (say .02") and a layer height (in order not to machine the full depth in one go).
These changes will however lower the accuracy for the ring's OD and ID, so add a third operation, with strategy Contour only and a tolerance of 0.0076"(D/33) to restore accuracy.
Some more tips:
- you need to set the Borders (Operation parameters) to "No extra": now you are cutting off the support tabs.
- I think you are using strategy Circular, unchecking sub-setting "Also machine corners" will save a lot of time.
Success ! Lex.
Thank you Lex!
This is very helpful in getting me started in the right direction.
Greg
Fiberglass isn't a good material for machining in the best of circumstances; I certainly wouldn't choose it for a first project. It's hard on tooling (diamond-coated is best) and on machinery. What are you trying to make? Can't you cut the wood and glass over it afterwards? If you really have to mill it, be careful not to let the dust get everywhere, particularly into the sliding parts of your mill, or your lungs...
Andrew Werby
www.computersculpture.com
Thanks Andrew.
I will do a practice cut on straight balsa first.
The final work piece will be 6 oz S-glass cloth layup over balsa (not G10/FR4 or filament wound fiberglass) and a Dremel will go through if fairly easy (just not very accurately). I am familiar with the dangers of cutting fiberglass (use a respirator, not a dust mask, vacuum debris, watch dust on clothes). But in this case it is a veneer (a couple of layers of 6 oz glass) that is bonded to balsa wood for a tough but lightweight composite structure. So I'm thinking that the milling shouldn't be that tough, since the initial layer is only about 0.4 mm (+/- 0.1mm). Knowing these things, do you think the mill will have difficulty with this or should I get cobalt bits for this kind of work?
Greg
Balsa is soft but stringy; it's not an easy wood to machine, even without fiberglass all over it. I don't think the mill will have difficulty, but the results might not be what's desired, since chipping-out is usual with this material. The cutter will get dull quickly cutting the fiberglass, and the polyester resin tends to clog it up. But it should work for a while. If you're doing a lot of this, diamond-coated tooling is recommended, as I mentioned. The main problem I foresee is that nasty fiberglass dust getting into the mill's moving parts and causing damage. Any fine dust will mix with the oil there and make a clay-like substance that tends to clog things up, but the glass fibers are also abrasive, so they're worse. Disassembling the mill and thoroughly cleaning out any residues after doing this would be good. If you can mount a vacuum cleaner nozzle close to the cut, that will help by removing dust at the source. A HEPA filter will help prevent it from spitting all that fine dust back into the room.
Andrew Werby
www.computersculpture.com
Andrew,
Below is a link I found for bits for composite cutting. Do these look suitable to the task?
http://www.niagaracutter.com/solidca...nd/diamond.pdf
Are there other bit vendors that you could recommend?
Greg
One thing I forgot is that is essentially plate stock, so no top milling is necessary.
How do I tell DeskProto to just mill the sides?
Greg
Set the segment height a little lower than the top of the part, and use a waterline toolpath strategy.
Andrew Werby
www.computersculpture.com
Thank you Andrew. That worked great.
Having all of the inside milled out is not necessary. Is there a way to just do the inner cut so that it forms a hole?
Greg
Hi Greg,
The area where no geometry is present is called the Ambient area.
You can use the option "Skip ambient" in order to skip that.
That will also skip the area around the ring though.
Lex.
Thank you, Lex. That works great for this work piece.
So the roughing looks good to me (first pic).
However, when I go to the finishing process (second pic), it looks like the milling depth goes way beyond what I want. How do I fix this?
Greg
Hi Greg,
These toolpaths are for a ballnose cutter.
Such cutter needs to go R mm (R=cutter radius) deeper than the bottom of the part in order to create vertical walls there.
Lex.