We are going to experiment with a 8 wheel WCD this summer, one question we have is how to mill the pockets in the 1X2 box tube to ensure that they are in the same location on both sides of the box tube.
Have teams created special fixturing to do this? We have a bridgeport mill to create the slots.
We have designed the bearing blocks to be two pieces, having a diameter of 1.5" that needs to pass through the box tubing.
Thoughts?
Kelly
You just mill them normally.
I wouldn’t recommend having the bearing block be round where it passes through the frame, it should be flat to spread the load across the wall of the slot.
Use an endmill that has a length of cut longer than 1" and machine the pockets so it cuts through both walls at the same time and make sure to take a light finishing pass (~.010")to get a good surface finish and to make sure there are no issues caused by tool deflection.
If you can go all the way through, do as said above and do at the same time. If you can’t, I would recommend you make some kind of stop or (ONLY DO THIS IF YOU HAVE STRONG TOOLS) using the tool with the edge at the 0 in the x direction and your 0 y be the stationary side of the vise, take out the part and slide it back in with the new side to machine in position so that it is exactly where is was before.
Now would be a good time to purchase some endmills with a 1"+ LOC. I understand doing this during crunch time when you don’t have any long endmills, but the middle of summer is hardly one of those times. They’re not terribly expensive either.
We have a gerneral rule of thumb that we machine as many operations in one setup. Anytime you flip a part you will induce error. Fixtures and tooling are great when you take the time to build it but that is a completely different design process.
You should no trouble machining those pockets in one setup with the same advice as the posts above stated.
My biggest piece of advice, square up the vice and the head. We do this multiple times during build season.
Realistically it makes no difference if you flip the part and end up with a slight offset (.010 might be the low end of repeatability if you very carelessly used a stop). Your vise is going to maintain the same Y zero (if you have no DRO and backlash it would be off a little, but it still doesn’t matter when you’re talking about a few thousandths), and the bearing block never contacts the X-wall of the pocket.
We machine ours through in one shot, but if you had to flip it you’re never going to notice the difference.
Any particular type of end mill recommended? Brand? Carbide vs. HSS? I used HSS last year, but never needed to have an LOC longer than 1/2". Is carbide the preferred alternative for rigidity in this case?
Also, maybe slightly off topic, but any recommendations on reference books/resources for workholding? That seems, to me, to be the biggest hurdle to get over. My team acquired a used CNC mill last year and while it took some time to learn how to operate it, fixturing was the hardest part.
We use carbide almost exclusively unless it’s a tool too large or uncommon to justify the increased cost. For small end mills the price differential is so small it’s not worth it to buy HSS. We purchase almost all of our end mills from lakeshorecarbide.com. Made in the US, very high quality/performance at a great price.
Fixturing was our biggest struggle when we first got our CNC mill. We kind of just got experience with it as we went and did more things. There are books I’ve heard recommended but they’re all $100-150. Practicalmachinist.com is a great site for metalworking forums. You can search for fixture designs or workholding tips and see a lot of great examples of how other users have done things, or you can get advice for your own parts you may be having trouble with.
Carbide is more rigid and can run at much higher SFPM, but your operation doesn’t really need that - pocketing in 1/8" aluminum should be pretty easy, and a 1/2" HSS end mill is going to be plenty rigid for almost all operations on a manual mill. Carbide is really better suited for CNC machines with higher RPM spindles. Just stick with a larger diameter tool with as little stickout as possible (to mimimize tool deflection). HSS is more forgiving anyway if you’re running the machine manually.
McMaster sells Niagara end mills, something like #2716A71 ($25) would be about right. The Lakeshore carbide end mills do have a good reputation, and are very reasonably priced for carbide tools ($48 for the ZrN coated 3 Flute EM).
Agree with Cory that using a workstop or indicating the part after you flip it should be plenty accurate anyway.
Carbide is better if your machine is rigid. If it isn’t, HSS will be more forgiving and less likely to break or chatter.
As for workholding, we bolt/screw/tape a lot of parts to subplates. The shop I work at does everything in at least 2 operations, typically milling the part out of a big block held in a vice, and then flipped over and held either against a stop or in soft jaws where the rest of the stock is machined off, and any other features are added. This does consume a lot of material, but your parts are a lot nicer.
We have a 1995 Wells Index 520…pretty good condition considering it was free. Seems to be fairly rigid…didn’t do any heavy machining (only <=1/4" aluminum plate or square tubing).
Last year for any tubing I flipped over the part and used a hard stop or indicated rather than milling straight through. I am intrigued though by milling the top and bottom of a, say, a 1x2 inch tube (through the 1 inch direction) rather than flipping. Sounds like a carbide endmill might be better (more rigid) for that sort of operation.
I have a few ideas about workholding. I have a vise and hard stop and it worked very well. Thought about getting a second vise to hold long pieces.
Another thought was taking a 1" thick aluminum plate that is wider/longer than my table and drilling/tapping a hole pattern for the clamps. The plate would be bolted to the table. This is response to a bit of trouble I had in making a part that is wider than my table, and supporting the ends that hang off the front and back (y-direction). The plate would also be sacrificial, so I could clamp the material right to it.
We have a lot of local jobshops who sponsor us in one way or another, and are a great resource for questions such as this whenever we get stumped.
The site Cory recommended is awesome, but nothing beats a local guy in the industry to stop by, see what you’re working with, and give you some pointers.
All of our mills have a massive piece of aluminum with 2 rows 1/2-13 for bolting vices and other clamps too without dialing them in. It’s really convenient, but it looks expensive to buy a piece of aluminum that big and ground flat.
This brings me to my second favorite metalworking supplier. Maritool. Fantastic prices on toolholders and pretty good deals on cutting tools. We buy all our collet chucks/end mill holders/milling chucks from him. Unbeatable for the price. No performance difference between his stuff and holders that cost 1.5 times as much. All his toolholders are made in Chicago in his shop. His collets are from overseas, but most of the rest of what he sells is made in the US.
That same half inch end mill (with 1.0" LOC) that you mentioned is only $4 more from Maritool in carbide. On a manual mill I wouldn’t bother with it, but on a CNC I nearly always find carbide to be a better choice and would pay 15% more any day.
The material itself is only half the price of something like that. The other half is the holes. making it flat is a few simple facing operations on a cnc mill.
I guess it depends on how precise you want it to be, and the layout of your machine, but I wouldn’t want a base plate that’s not ground flat.
Most machines have a substantially larger table than travel of the machine. Unless you have a large fly cutter you can’t machine the entire surface in one shot.
As soon as you clamp or bolt the plate to the table to take a cut and flatten it out you’re introducing/relieving stress as you clamp/cut/unclamp. As long as you’re clamping it you will never truly get it flat while milling it.
If you clamp it and machine it flat and leave it in place and never remove it, it will be flat, at least as long as your machine is perfectly leveled at the time you cut it, and it never changes level after that.
In all likelihood the last method is probably good enough, especially if your machine is older/worn out.