Workholding for contour of parts

[Pharkas]

Hi,

I'm fairly new at this.

I have to mill the contour of a part, 0.375 thick in A36 steel.

There are no holes in the part so I can't use bolts in the middle to hold the part down, which is how I usually do contours.

How would I hold this piece down for machining ?

Thanks !

[widgitmaster]

In the past I have run contoured parts using two vises, one had hard jaws, the other had soft jaws.
First vise would hold the mill stock blanks and machine the top side of the part.
Then the 2nd vise had been contoured into the soft jaws so the part would nest perfectly around the contour! Then the machining of the 2nd side was done.

This way, every cycle start you would get one complete part.

-------------------------------------------------

The other method is a little more costly, as it requires an extra length of stock preferably round, and the part was held in an indexing fixture using a three-jaw chuck.
When all the machining was complete, the extra knob was parted off in the lathe.
Either of these methods will work on regular sized CNC milling centers.

Hope this helps!
Eric

[Geof]

Is this .375" plate? I have done contours around flat pieces using two sets of clamps and two versions of the program. Have the first program lift the tool to jump over the first set of clamps, then install the second set of clamps where the contour is finished, remove the first clamps and have the second program jump over the second set.

[spyder]

try this product solidmax web www.solidmax.org

[mxtras]

The above methods by Widgit and Geoff are good to use. I usually will clamp outside the contour if possible then cut through the profile all around except in two or three stratigically placed areas where I will leave a very thin tab to hold the part to the stock. After the profile is complete, pop it out of the skeleton either with a mallet or a pair if snips (or a chisel, or?) and the small tabs left on the part are removed with a beltsander, file, snips - whatever. Adjust the size and thickness of the tabs to suit your needs. I usually leave around 3MM wide tabs that are maybe .15mm thick for aluminum parts - for steel you will have to be a bit thicker and maybe slightly larger. I position them in an area that is easy to get to with the beltsander - like on an outside corner. The position of the tabs is dependent on the shape of the part, your starting point and your tool path but their placement is fairly intuitive.

Scott

[fpworks]

I'll throw another technique out there...cut off the part with a saw in the spindle. It is a useful alternative when you have small parts and there is a lot of remaining [difficult] material that you don't want to machine away.

I used this technique to part off some 1" x 0.25" x 0.25" contoured parts that I made in M4 tool steel. There was almost another inch remaining of the clamping butt, so I used a thin carbide saw to part them off.

The saw will leave a poor finish, so I left 0.3mm of stock for cleanup. I then went back and I made a set of contoured jaws machine the bottom of the part to height and added a chamfer.