[chris123]

I need some help
I have a CNC mill and I'd like to mill both sides of a object
Does anyone have any pointers, tips, tricks on how I can align the part correctly after flipping it over?

[whitehedr]

If you have a through hole you can use that to locate the part after you flip it over. I chucked up the drill bit that was used to make the hole and then
located the part by placing the through hole on the bit with out moving the vice or table. I don't know if that is an acceptable machine shop practice but it worked for me.

RWW

[SirSmash]

You'd have to keep something on the part to align with, like whitehedr said a hole works well... Keep some extra material on a corner to place the hole, when your done you can cut that extra bit off.

You can also make two halves, say you're making a horse or something, and glue them together once you're finished.

[chris123]

The part Im making is an aluminum part about 1.5"x1"x0.3"

If i flip the part around the x or y axis wont bottom become top or left become right and I'd have to move something in order to align the hole with the tool bit?
I'm using visualMill and EMC2
So you saying I add an extra side bit with a hole to the model and machine that.
How would I get the z-axis aligned?

[Fastest1]

Definitely build a simple fixture plate to hold it down on. Then as mentioned above have a thru hole. Try seperating your routines so you can move clamps from inside to outside or from 1 pocket to another. When relocating your part/flipping it over, try running the bit slowly in feedrate with the spindle off and make sure it is aligned as close as possible. Regarding machining practices, I am not a machinist but I did hear something a while back that stuck with me, if you can hold it safely and perform the functions you need, it is correct. I always figure out a way to do it easier, faster and with better results during the 1st set up and constantly after that. If I have time or need I would refine them. But holding that part down firmly and indexing it is critical. I have hand wheels on my steppers and have been known to turn the controller off and run the axis' to where I need it or think it belongs and then repower. I am sure there is another/better and or smarter way but I dont know it yet and this lets me move forward! Good luck to you and lets us know how it works for you. I just did my first 2 sided part, a simple bracket to those with experience. Results werent great but not too bad, the friend who needed it thought it was great. I do know how to make it better and will do it as a personal challenge and gift it to him as an extra. However his design sucks and I am also going to totally redesign another bracket and clamp for him. It will be simple,stunning, light, durable and easy to use. It is going on a flattracker, those guys dont know how to build anything pretty, just strong.

[chris123]

I've had my mill for about 5 years but never did much with it
I'll machine something simple see what happens
I don't have a problem milling the part from the top side, it looks great. I just need to be able to turn it and get it right and aligned on the other side

[BobWarfield]

RE the alignment, you can certainly use some feature on the part as your datum, but it is a nuisance to have to go line it up with your edgefinder, coax, taster, or whatever.

Workstops are your friend for making this stuff fast. If you can arrange to use stops of some kind you can flip the part, place it against the stops, tighten the vise and go.

When I do my CAD, I do the drawing so the part is aligned below 0,0 on the positive x side. That means my vise's fixed jaw's lower left corner is 0,0. That vise doesn't move around the table very often, so normally I can walk in, home the machine, slap a part in the vise, and go. When you flip the part, make the same assumption. 0, 0 for the program is that corner of the vise jaw. It's often worth it to do a separate CAD drawing of the bottom just to keep everything clear. Easy to produce that drawing from your 3D model too.

The other approach is soft jaws, which are also great, but you have to spend time making the jaws.

Cheers,

BW

[chris123]

I think my problem is I dont understand most of the terms used or how that would work
OK read up on workstops
I kind of understand, I should actually try these things in practice first before commenting
How about if I just buy a 4th axis....

[Fastest1]

You should be able to invert or flip the part in your cad side and keep the hole location as the reference. I think. I know there are people who can do that. Fortunately my part was symetrical.

[BobWarfield]

I think my problem is I dont understand most of the terms used or how that would work
OK read up on workstops
I kind of understand, I should actually try these things in practice first before commenting
How about if I just buy a 4th axis....

Chris, you want things like workstops to be second nature before you start wrestling with a fourth axis. It's a whole other level of complexity and programming.

Best,

BW

[knudsen]

http://books.google.com/books?id=R7F...0setup&f=false

http://books.google.com/books?id=6UF...0setup&f=false

If the first two don't put you to slep, one of these will:

http://books.google.com/books?q=rela...rbooks_s&cad=1

:rainfro:

[CMSGlassGuy]

Along the same lines, you can create/machine a mated fixture on the machine for the part.
Step 1: Use Cad to create part + a two phase fixture that is machined while pinned to the cnc table so that all datum references are dead on.
Step 2: Locate with rough sides A & B in fixture phase 1 area, machine sides C & D
Step 3: Locate sides C & D into mated fixture phase 2 area, machine sides A & B

The part should be programmed in CAD as it will be located on the fixture. I do all of the work in one project and then save it off as difference operations without moving anything.

The "mated" elements of a fixture can be a machined 90 degree corner or a complementary shape. If using an inside corner, be sure to make a small relief cut into the corner itself to remove the inside corner tool radius, allow for dust and let the corner of the part seat completely.

Fixture materials can be MDF, Plastic, Aluminum..
Add clamps and or vacuum channels and gaskets as necessary.
Once you understand fixturing, it will greatly expand you capabilities.
Developing standard practices will help your operator understand what you are trying to accomplish, add efficiency and saftety.

[chris123]

I beleive I shall do some reading first

[Fastest1]

Very well said and the fixture is also partially sacrificial so cutting it instead of the table is a good thing at least in my case. It also allows full depth cuts and dont forget to watch what the loose parts will do once free.

Along the same lines, you can create/machine a mated fixture on the machine for the part.
Step 1: Use Cad to create part + a two phase fixture that is machined while pinned to the cnc table so that all datum references are dead on.
Step 2: Locate with rough sides A & B in fixture phase 1 area, machine sides C & D
Step 3: Locate sides C & D into mated fixture phase 2 area, machine sides A & B

The part should be programmed in CAD as it will be located on the fixture. I do all of the work in one project and then save it off as difference operations without moving anything.

The "mated" elements of a fixture can be a machined 90 degree corner or a complementary shape. If using an inside corner, be sure to make a small relief cut into the corner itself to remove the inside corner tool radius, allow for dust and let the corner of the part seat completely.

Fixture materials can be MDF, Plastic, Aluminum..
Add clamps and or vacuum channels and gaskets as necessary.
Once you understand fixturing, it will greatly expand you capabilities.
Developing standard practices will help your operator understand what you are trying to accomplish, add efficiency and saftety.

[chris123]

I've completed making my first 3D part
I was x and y are correct but I was out in z-axis by about 1mm, either during a tool change or the part moved
I am going to reference the bottom of the clamp this time and also lock the the part in better

[Fixittt]

I do some large plastic parts. I built me a fixture. Thing solid flat plate with 2 pins. One on each end of the plate in line with each other.

I bolt this plate to my table and indicate it square using the pins. If both pins are centered along my X axis then I now have a known location. Find the center of the pins and Zero Y to this location. Dray your part with the Y zero in the center of the part. I drill holes in my 1 inch thick plastic and use the pins on the fixture to bolt down the material. Cut the top. Unbolt the material, flip and place it back down over the pins. Bolt down then cut the back half. But yes, if the part is not symmetrical, you have to rotate the cad drawing so that ever thing lines up.

[chris123]

My replacement part did fit but i broke it, as I expected. The side walls end up being just a few mm thick and I made it in pine
I also don't have a rigid enough tool to bore the required hole deep enough and wide enough, the cylinder that slides inside just forced it apart and split the wood at the far narrow end

[ViperTX]

Well here is what I do....when I use MeshCAM I center the part on the stock, so when I flip it over it should be aligned.

I have straight edges on the x and y axis that I use and my stock is always rectangular.

Paul

[chris123]

My stock is cylindrical, turned, bored and mostly complete, it just needs the end milled
I center the part in the stock on the CAM program
I clamp it in a vise and hold the stock down with another clamp
Center the mill to the top edge and mill
I should make a jig so when i rotate the part is rotated 180 degrees
The I mill the other half