How can I machine this?

I am trying to make a pulse jet engine with an argus type valve. Below is a picture of one of the reed valve retainers. These are the most complicated parts (geometry wise) in the entire engine.

The part will be machined out of 5/8in thick 1.5in wide aluminum bar that will be cut to the proper length prior to machining. Those are the exact external dimensions of this part meaning that the machining should ONLY be done to cut out the holes, channels, and other features there should be no tool pathways around the perimeter of this block.

The only machine I have is a Fireball V90 cnc router with a Bosch colt router on it. I have metal cutting endmills and ball mills for it as well as a spray mist cooling system hooked up to it. This machine is more than capable of machining aluminum with shallow passes.

http://img832.imageshack.us/img832/2...vesnapshot.jpg


Now the part is double sided but that is not the problem. My main issue is cutting the angled cuts which are CRITICAL in the functionality of the pulse jet.

I have pointed arrows toward the problem causing cuts in this picture.


http://img861.imageshack.us/img861/2...vesnapshot.jpg



This type of part is something that I would be able to machine immediately notice there are no angles. This would be simple to set up in cambam.

http://img828.imageshack.us/img828/7454/partrender.jpg









DOES ANYONE HAVE ANY IDEAS??? I would really appreciate any input

I have attached the STL file for this part if dxf files are needed I can post them as well. I opened it just fine in the latest version of Cambam.

thanks.









.

Post this on the CB forum, I'm sure the guys there be more than happy to help and they know CB like back of their hand.

CamBam - Index

Smooth90

You are correct, machining the part without the angles is very easy in CamBam. You could even machine the part using waterline rough then waterline finish which would give you a smooth finish on the horizontal and vertical surfaces. However you would be left with tiny stepped toolmarks on the angled surfaces. What I would do is use the waterline rough/finish steps then, build a 'jig' to hold the machined piece so the tapered surfaces are parallel to the work surface, then just do a surface pass to smooth the fine tool marks left by waterline finish. Obviously, this would have to be done for each side but it will get you what you need.

Don

I thought about making a jig although making one will be tricky. Since I can't mill at an angle to make a perfect jig I will have to create an angled jig from flat parts.

Recently I added an awesome tool to my shop that will make this really easy......a miller diversion 180 ac/dc tig welder. This will enable me to weld aluminum together.

I plan on cutting about 4 aluminum triangles out of 1/8in sheet. I will then weld an 1/8in strip (say 2in wide) to top of those four triangles. When placed underneath the part I need to mill it will cause the angled surfaces to become parallel to the work surface.

These parts will probably take 3 hours a pop to mill and I've got to make 4....err I wish I had a proper milling machine!

Smooth90

That approach should work fine.

Don

Ok so I whipped up a jig that will allow this to work. I have to do some more work to make sure that the top plate that holds the part is perfectly level otherwise the cut will be thrown off. I will do this by making a depression on the triangular mounting pieces for the top plate to fit into and by . Once that's done its just a matter of welding those triangular pieces at a perfect 90 degree angle.

My plan is to take the aluminum block and use cambam to machine the 2 holes into it as well as a mark as to where the angled notch has to be. This will allow me to attach the block to the jig with bolts. Since the angled surface is now parallel to the cutting head I can use cambam just like if I were maching flat notches into an aluminum bar. Once I line it up to the notch that was made and verifying that everything is level and in line I can run the cnc and have it machine the notches into the bar. Once thats done I can flip the bar over and machine the notches on the other side. Once the angled part is finished I can actually use cambam with flat 2d dxfs to finish making the channels and other features. Then hopefully in the end I should have the finished part....repeat 3 more times and I have enough parts to build the valve.

Here is some renders of my jig so far.


http://img535.imageshack.us/img535/6564/jigpic1.jpg


http://img225.imageshack.us/img225/9448/jigpic2.jpg

I can't understand why this can be machined in CB using 3D function with out any fixturing. Just use appropriate ball mill. You also would have to polish the hell out of this parts because of little groves created by the endmill, but this would be it. My 2¢:):)

CamBam is quite capable of generating the 3D code for this piece, however, even using a ball end cutter there will be small grooves that need to be polished out as you said. Also, there is a 90 degree inside corner on the end pieces that cannot be cut with a ball end or even an end mill without setting the piece at an angle to get the 90 degree corner. Now, if one had a 4 or 5 axis mill, then no sweat. ;)

Don

if you used a .125 flat bottom endmill to cut your angles you will only see .007 of the fillet in the corners

Very good point Don. Somehow I overlooked the outboard steps :D. It all depends how critical those steps are. If it's working surface then is a problem if it's only clearance/relief surface then I say don't worry about it.:D:D

If you wanted to mill it without a fixture would you not do as much of it as possible in CamBam then write 1 or 2 subprograms that milled those angles? Start above them and feed down on that angle and loop it at the increment of the centers of them. Then on the lower part write it do it will step over 3/4 of the cutter or something and start above the angle and mill down.

I think the jig is probably the only way for you to do this properly and keep the sqr corners. If you had a 4th axis now that would be another thing.

Steve

So, how did you end up doing it? Out of curiosity, and because I have a similar project in mind.

There is a plugin for cambam for cutting flat, round and sloped surfaces in 2.5D.
you can find the plugin in the scripts and plugin area in the cambam forum, the name is "Curved Surface Plugin for CamBam"

ralf

I think CamBam don't support plugins.

CamBam supports plugins and scripts.
A list of existing plugins you find in the forum

ralf

Quote:

---

Originally Posted by youssefedward

I think CamBam don't support plugins.

---

There are tons of plug-ins for CB. Some of the current features are past plug-ins. While it has a primary design team of one lots of users write plug-ins for various things. One of my favorites is the thread milling plug-in.

As to the original project posted. A jig is certainly the best way to cut the part in my opinion, but 3D machining would work with the limitations mentioned. It could also be done with 2.5D machining as CB has a native ability to profile with an angled side wall from a polyline.