Tabs on part while milling

I need to machine a part that looks something like my sketch. It's .625 thick alum. And it's roughly 3x4". I need to do both inside cutting and then cut the contour. I was thinking to load a bar on my table long enough to make say 10 parts. Machine the inside of each then cut the outer profile. And if possible leave a .25 wide "tab" on two sides maybe .200 thick to keep the part in place at the very end. Then just sand it off when done.

Any pointers? Or ideas? I want to nest them to save on material instead of band sawing it all into blanks ahead of time.

Also is there any slick way of making the "tab" in BobCad?

Thanks!!!

I would think you will need three tabs to keep from getting too much vibration.

I would start with 3/4" thick bar, hold it by the bottom .090 or so, do all the inside and the profile, then facemill the backside off to 5/8". Maybe stagger the parts so the ears are opposite to save material if you have a large quantity. Multiple vises, two parts per vise. Why do you need tabs?

ZachN said:

View attachment 122799

It's .625 thick alum. And it's roughly 3x4". .... if possible leave a .25 wide "tab" on two sides maybe .200 thick .... Then just sand it off when done.

I want to nest them to save on material instead of band sawing it all into blanks ahead of time.

Click to expand...

Pointer1: Bandsaw kerf is about .05 thick, with allowance it's .1" - Can you machine 5/8 thick with a 3/32 endmill?

Pointer2: What is the sanding time going to cost? Yes, sanding belts are cheap to the point of no consequence, but .... the result will be ugly.

Pointer3: What is the dimension between the two flats?

About pointer 3, if you are conscientious about material cost, then jkruger's idea won't work as you'll waste 1/8" of material, but you will
gain with a dead nuts part that is pretty and unquestionable ( this would be my preferred method of doing this BTW )
If OTOH you can live with an extruded surface, then buy rectangular 5/8 stock that is oversize, saw cut to slightly over the width, mill both sides and inside profile
in sacrificial soft jaws and then add a simple facing operation to bring the flats within tolerance.
That is how I make the " I don't care, it's just a simple bracket that works" parts of similar ilk.

Your idea will work, but you need to leave a "frame" of material around each part. The frame provides support while you are machining. The tabs can be very thin (< 0.02) and they will still be remarkably strong while attached to the frame. This technique is more about saving time than material.

This is something I do all the time (and am going to be programming my next part for), but I usually leave a complete membrane rather than use tabs, it depends on the geometry and the stock I'm working with. If it's a membrane (complete perimeter), I'll leave ~.006 for a thin part (< .250), .008 or .010 for a thicker piece. At these thicknesses the part can be (carefully) broken out of the stock with a soft hammer, sometimes using a utility knife to cut sections of the membrane first. The edges left can be pealed away with a pair of pliers, just don't cut yourself with the waste as it pulls off. Depending on part geometry I'll tumble the narrow remaining edge off, sand it, of take a light facing cut.

If I use tabs I do make sure there's at least three, but they can be pretty small and thin at the final cuts so that they're easy to break free. I just add them manually into the CAM file, with my software it's easy to do with a few line breaks and height changes as I work.

A note on jkruger's comment - I try not to leave that much material, due to the waste/cost of the extra metal that gets turned into chips, and because many rolled materials have stresses in them that can come out when asymmetric cutting is done. If you've pocketed one side of the part, then face off a bunch of metal from the other, you're almost certain to get some stress relief resulting on distortion of the part. A thin cut (<.010") is less likely to have this happen.

If YOU want tabs you can buy the nesting feature with BoBCAD.It will have the option.
If YOU learn the basics of 2D CAM,you will be able to do it yourself.
If YOU do a search on the BoB Forum at the other place,you will see it has been discussed many times.Many ways offered on how to do it.

If YOU want a good looking part to print,each and every time,,,do the sacrificial 1/8 inch that jkruger suggested.That's the way I do it.

I use the waterjet for those parts.
Have you thought about sending them out to get cut? Might be more practical depending what they charge you. Just a thought.

This video shows how V27 and nesting works to leave tabs.


You other option would be to break the profile to leave a section that is un cut. Where you the users changing the part profile to leave a tab. Also the flip and face method works too!

If there is anything else I can help with on this topic please let me know.

Draw it in 3D wireframe(with tabs),,machine it with 3D engrave(outer profile)

ZachN said:

View attachment 122799

I need to machine a part that looks something like my sketch. It's .625 thick alum. And it's roughly 3x4". I need to do both inside cutting and then cut the contour. I was thinking to load a bar on my table long enough to make say 10 parts. Machine the inside of each then cut the outer profile. And if possible leave a .25 wide "tab" on two sides maybe .200 thick to keep the part in place at the very end. Then just sand it off when done.

Any pointers? Or ideas? I want to nest them to save on material instead of band sawing it all into blanks ahead of time.

Also is there any slick way of making the "tab" in BobCad?

Thanks!!!

Click to expand...

I do the same thing quite often.
After milling, I cut the tabs on the band saw and clean the edges with a belt sander.
Add the tabs on a straight edge or the outside of a curve where they are easy to get to with the sander.
I usually go with at least three tabs spaced around the perimeter. Not much of an issue if you are milling on a spoil board. If your are holding parts off the table in a vise, the part can rock when only suspended off a couple of tabs.
If the part is aluminum, the tabs can be full height. It is just as easy to sand a short tall tab off as a low wide partial tab.
For simple parts like this, I use V-carve software. The built in drawing program adds tabs almost automatically. The biggest problem with using tabs is that the bit will ride up the tab and down and it can leave tool tracks in the edge material.
Dennis

All good ideas! Thanks! I think I'll go with 3 full height tabs and give it a shot.

Sending it out, yes I thought about that, but it's nice to make any change to the design in house after 1 part is made and not 500. That's the huge factor that's very unique to our business in a way. We are testing the function as we go sort of speak.

Nesting with BC looks like a good option down the road. Looks like I'll add that to my upgrade list.

Milling the face off of thicker stock was a good idea till I notice the price change in stock cost and stress relief is also a concern. They can't warp or I'll be in trouble.

I'll find out in the next week or so when I try to tackle this project. I'll try my best to remember to post an update.
Thanks guys!

I use a router with a flush trim bit to trim tabs when I use them.
Jordy

ZachN said:

.... and stress relief is also a concern. They can't warp or I'll be in trouble.

...

Click to expand...

If you think that the warping on a 3 x 4" piece will be more than your sand-belt-offing of the tabs, then you ARE in trouble.

SeymourDumore said:

If you think that the warping on a 3 x 4" piece will be more than your sand-belt-offing of the tabs, then you ARE in trouble.

Click to expand...

I kind of agree. While I wouldn't have thought the part would warp at all (could be wrong), I definitely would not think the part would warp with a little bit of sanding. But then again, I don't usually have any parts that would be an issue in that sense. I suppose picking the "right" aluminum would help in that aspect. Maybe 6061? Again I'm not a pro in that dept

ZachN said:

Milling the face off of thicker stock was a good idea till I notice the price change in stock cost and stress relief is also a concern. They can't warp or I'll be in trouble.

Thanks guys!

Click to expand...

A few cents spent on material can be better than spending machine time puttering around with tabs. Tabs require a lot more tool time to enter and exit the cut, unless, by some miracle, you can simply withdraw to clearance, and move across the tab, then plunge in and keep on cutting. Plus, you are wasting stock around the exterior of the part. Using the 'thin skin' method, you can cut barely larger than part size, hold the stock in TalonGrip jaws and machine around it. Cutting the 'carrier' off is better done with a chamfer operation on the reverse side, but you'll need a proper soft jaw to locate the part for the trimming operation.

But, you do need two 'quite parallel' edges for TalonGrip to work properly.

HuFlungDung said:

A few cents spent on material can be better than spending machine time puttering around with tabs. Tabs require a lot more tool time to enter and exit the cut, unless, by some miracle, you can simply withdraw to clearance, and move across the tab, then plunge in and keep on cutting. Plus, you are wasting stock around the exterior of the part. Using the 'thin skin' method, you can cut barely larger than part size, hold the stock in TalonGrip jaws and machine around it. Cutting the 'carrier' off is better done with a chamfer operation on the reverse side, but you'll need a proper soft jaw to locate the part for the trimming operation.

But, you do need two 'quite parallel' edges for TalonGrip to work properly.

Click to expand...

I can perform that miracle,haha,,,,,but due to the nature of what I do,there is always a better solution than tabs.
I can certainly see times when millingtabs could be beneficial.
I know of many ways to do this and hinted at some of them.It has been discussed many times at the other place and I pointed the OP that direction.He should be able to surf over there if he really wants an in depth understanding of BoB and Tabs.
Couple guys even wrote scripts to do it.