Seeking advise. Brother + orange vise + Sandvik facemill

sage9984 · Jan 15, 2019

Please see the video at the link.

https://youtu.be/tNY2T7gmtw4

The face mill is used for op2. I'm using it just for cleaning up the back side from op1.

DOC is 0.06". Sfm is 1500 and feed is 35 ipm. Stepover is 1.2" and and part width is 2.25".

Final thickness needed to achieve is 0.312". I'm holding 0.290" inside the jaws. I am holding about 0.250" inside each jaw.

The problem I'm seeing is after I unclamp the vise and measure the part, I get 0.313" on either side of where I'm holding from the jaws. In the center area approximately the width of the center hole, the thickness drops to 0.310". Can anyone advise what I am doing wrong?

Finegrain · Jan 15, 2019

Aack, I about fell asleep watching that :crazy:

. Please tell me you had everything slowed down just for the video.

Vise could be popping the middle of the part up, even though it's almost a full-depth grip. Also possible the facemill is pulling the part up, but I doubt that is happening at that slow a feed.

Are you sure the P1 face is flat? The part might have been bowed during P1 due to vise pressure.

Regards.

Mike

D.D.Machine · Jan 15, 2019

sounds like its bowing up ... turn the part 90* and re cut it and see what your getting ...

Or

put in indicator in the spindle and see what the part does when you tighten the vice ,,,

Are you starting with flat bar or plate? I have found flat bar seems to move around more when you cut it ,,, I think it gets more stress in it when they pull it .

sage9984 · Jan 15, 2019

P1 is machined with talon grips.

sage9984 · Jan 15, 2019

Starting with bar stock.

D.D.Machine · Jan 15, 2019

cut the first side then check for flat ,, then clamp and reach under side of clamped part and recheck bottom surface for flat ..

You could be putting stress into it on first opp clamping , or on second opp clamping ... you might want to use a torque wrench to tighten the vise ,, I do a lot of alum plate work were I have to use a vary light grip ..

Finegrain · Jan 15, 2019

sage9984 said:
P1 is machined with talon grips.

I use Talon Grips on most production jobs. They are great, but can definitely bow your stock. I bet this is where that .003" went.

When you grip your stock for P1, torque the vise down hard such that the grips create divots, then release the vise, and retorque quite lightly, like just snug. The grips will seat into the divots, but won't bow the stock. You can put an indicator on the top of the stock to get an idea of how much bowing there is.

Regards.

Mike

sage9984 · Jan 15, 2019

Ok, will have to check that tomorrow morning.

Hazzert · Jan 15, 2019

I’m having a hard time visualizing how he’s describing it...

If your part is thin across in the X then it is your clamping pressure or stock removal in Op1 or 2. Take one over to the granite table and set it up on three points with the 4 corners level and see if your Op2 side is responsible for your dip or not.

If it is, put an indicator on the part when you clamp so you can see if your puckering it. Adjust clamping pressure until it’s something you can live with ornthe parts stop flying out of the vice, whichever comes first.

If it’s your Op1, try what Finegrain suggested and release your clamping pressure once you divot the stock. I’d also be inclined to poke the hole in the middle before facing with a unclamp reclamp in between but your talon jaws would just stress the stock again.

Matt@RFR · Jan 15, 2019

The tighter you clamp with a vise (any vise), the worse this problem becomes. This is what surface, blanchard and double disc grinders are for. You can get it flatter in the mill, but perfection aint happening.

When you sink the talon grips in to the part, loosen the vise again and then just barely tickle the part with the grips. It can't go anywhere. As for op 2, people seem to clamp the fuck out of everything when it's almost never needed. Try taking it easier on the clamping force. It won't cause total devastation if you sneak up on it... you'll see the part thickness start to move when you're too light.

Freds · Jan 15, 2019

How wide is the 'lip' of material (distance from finished side of part to talon grip)in op1? Do you do the facing of side one as the first op or do you come back and hit it after all the features are added? Given that you are facing off 0.06 in op2, op1 must be right on top of the talon grips; if the lip is more than, say, 0.100 wide, part might be unstable for later ops of first setup.

Fred

nscele · Jan 15, 2019

That's an issue using a double station vice where one op is roughing needing clamping force and the other op is finishing using less force, I do a couple of jobs also on an Orange double station vice and can very easily bow an 8mm thick plate by tightening the vice too much.

gkoenig · Jan 16, 2019

You bought a Speedio... why are you running it like a Slowio?

- Faster with the face mill
- Eliminate all that wasted motion on the spotting drill.
- Ditch the feed height in HSM/Fusion

This is what it should look like:
Brother speedio s7x1 - YouTube

You're getting the part bowing because of the clamping pressure on the vise. Clamp the vise just barely in contact with the part and throw an indicator on it. Then tighten the vise down... you'll find the 0.003".

Best solution if it is possible? Less clamping pressure on the vise. One trick is to tightly clamp the vise so the Talons bite on the stock for Op1 and create their indents, then loosen it and clamp with a torque wrench to *just* enough for a reliable grip on both parts. The initial Talon bite will indent the raw stock and let you use significantly less overall clamping force (sort of like the Lang stamping grip thing).

If there is still too much clamping; you could make a quick and dirty miteebite fixture and keep it in station 2 on the vise against the stop. More elaborate ways to do it (like machining a fixed jaw for the Orange that has talon grips on one edge, and the pallet with the miteebites holding Op2).

sage9984 · Jan 16, 2019

Hey thanks for the advise. This is my first setup on the brother and first ever milling job. I don't actually know all the terminology. I am still learning even just the basics. I am strictly a screw machine/CNC lathe shop. This is our first cnc mill for production.

Mtndew · Jan 16, 2019

sage9984 said:
Hey thanks for the advise. This is my first setup on the brother and first ever milling job. I don't actually know all the terminology. I am still learning even just the basics. I am strictly a screw machine/CNC lathe shop. This is our first cnc mill for production.

1st ever milling job and you have one of the fastest machines on the market. Damn. I'd be going slow too!

Insert · Jan 16, 2019

If you do all what the others have mentioned, and you are still getting a little bowing, add that big hole last, your cross sectional area is the smallest at the worst possible location.

Finegrain · Jan 16, 2019

If all else fails and you still have a couple thousandths difference, split the difference between the middle and the edges. You'll be .0015" off instead of .003".

Regards.

Mike

gkoenig · Jan 16, 2019

sage9984 said:
Hey thanks for the advise. This is my first setup on the brother and first ever milling job. I don't actually know all the terminology. I am still learning even just the basics. I am strictly a screw machine/CNC lathe shop. This is our first cnc mill for production.

Oh shit dude... Did you also get you’re driving learners permit in a Porsche?

I withdraw my snarky humor!

coffeetek · Jan 16, 2019

Yeah, that's vise bowing the part out in the middle from too much pressure. If you use torque wrench, experiment with torque and measure the bow you should be able to get <0.0005" On few of my parts I need to be at 0.0004" or less over 3" diameter and its possible but you have to be very careful.

droshi · Jan 16, 2019

I had a wide (4") part that was only 1/4" thick stock. Holding it in a vise can work, but using a face mill like that it puts a lot of downward pressure. You could try using a 3/8" end mill and see how facing goes, it should put less downward pressure on. I ended up making a pallet to support my piece entirely from the bottom with two Pitbull clamps on one side and a rail on the other.

I have a similar setup as you, except I'm using an 80mm Sandvik 345 mill, can't tell your model exactly from the video, but I would guess it probably puts a lot of downward pressure. I have a Century mill on my list to pick up one day and see if that's any different. For your part on the facing, speed/feed will depend on your material (didn't catch what it was?), inserts, mill type and how many flutes. So more info would help a lot, but as a guess you could probably easily double your feed rate at least.

My advise would be to mill you some soft jaws that support the under side of your part a lot better.

FWIW I keep my Speedio on 4 for rapids, I didn't buy it for the speed personally. I'm sure it will be nice to have, but since I do a lot more prototyping than production, to me the maintenance was the reason for buying. No need to be tempted by the speed demons out there. I personally just think run your tools at around 80% of manufacturer recommendations depending on who they are...some will give you blistering speeds. Others give very conservative. Once you figure which is which, you can adjust from there.

Seeking advise. Brother + orange vise + Sandvik facemill

Plastic

Diamond

Stainless

Plastic

Plastic

Stainless

Diamond

Plastic

Stainless

Titanium

Cast Iron

Aluminum

Titanium

Plastic

Diamond

Hot Rolled

Diamond

Titanium

Aluminum

Aluminum

Similar threads