Milling nested parts from steel plate... design issues??

[InspirationTool]

So, I've been doing alot of designs that are 2D in sheet metal and having them cut on laser or waterjet. Nesting and workholding is a piece of cake in this situation. Cheap, fast and effective.

Now I'm looking at doing some designs in 1/2" or 3/4" steel plate, with 2.5D features and higher accuracy needed than I can get with laser or waterjet. Obviously to me this means vertical mill.

Let's say I have several non-rectangular shapes with interior bolt holes to cut out of a 12" x 24" 3/4" thick steel plate. Say a run of 10 plates worth. How would you guys go about doing this?

Can you just clamp it to the table with a sacrificial sheet underneath and "tab" it in like you would a piece of plywood? How do you then cut the part out?

Do you make a bolt-hole specific sheet underneath, cut the bolt holes, bolt the parts down, and then cut the parts out?

Mitee-bite clamps? Standard bolt-hole pattern?

I'm wondering if there is anything I can do to make it easier and cheaper to manufacture parts when I design them.

Thanks!

-Jeff

[Geof]

Where is your higher accuracy required; bolt hole size and location or in other places on the parts? I suggest you look at using both laser/waterjet and vertical mill. Cutting parts directly out of a sheet of 3/4" material on a mill is going to be slow and as you realise workholding will be difficult. You may find it best to get them cut with a machining allowance and then finish them to the precision you need on the mill. This allows you to solve your workholding problem because you have bolts holes available. If the bolt hole size and location tolerance can be met by the cutting method you probably need only one fixturing for the final machining. If the bolt holes need to be brought to tolerance you will just need to have a stop in the machining program and use only some of the bolt holes for fixturing with the program working on the unused ones.

[mrainey]

Do you make a bolt-hole specific sheet underneath, cut the bolt holes, bolt the parts down, and then cut the parts out?

Without knowing what the parts look like or what tolerances you're trying to hold, that sounds about like what I'd try. Particularly if it's going to be a repeat job.

Make a base plate with two or three tapped holes from each bolt circle that will be in your nested plate. If you had twelve parts, you would have 24 or 36 holes in your base plate.

Drill all the holes in your nested plate, then bolt the nested plate to your base plate and machine the profiles.

[InspirationTool]

The hole locations need to be more accurate than the outside profile with some holes tapped and some reamed.

It soulds like I could waterjet cut some extra holes just for use as bolt-down locations and then machine the other holes and the perimiter in one shot on the mill.

I guess the other option would be to design the part to use standard size rectangular stock whenever possible.

Thanks guys!

-Jeff

[Geof]

Originally Posted by InspirationTool .....It soulds like I could waterjet cut some extra holes just for use as bolt-down locations and then machine the other holes and the perimiter in one shot on the mill.....-Jeff

I think this is the best solution. We do it on some parts we make and the only disadvantage is sometimes a customers phones to say they put such and such together but they could not find any use for two or three of the holes; did they do something wrong?

[NC Cams]

We use "masters" to grind cams - basically a precisely milled "washer".

A CNC unground "master blank" costed us roughly $45 from a dedicated supplier.

As a SWAG, we took 3/8" HR plate and laser cut out a blank ( basically a washer) with 5 additional and properly spaced bolt holes that we use to bolt it down to a fixture with countersunk allen bolts.

The holes roughly index the part to within 0.010 or so - we have 0.05" stock left for ID machining. The OD is unmachined which we do with a CNC to whatever form profile we want/need to make.

Once the plate is bolted down, we use a CNC cutter to "tune up" the the laser cut piece (ID and indexing slot) to within 0.0003" or so. Same effective part for a fraction of the cost.

Cost is about $9 for the lazered blank in bulk (including material!!!) and about 15 min to do the milling tune up. At $80/hour, the laser cut "blanks" net out at about $25 each versus $45 for purchased ones.

In summary, use the laser or water jet to hog/rip out the blank and then use a CNC to do the subtle precision/finish machining ONLY as needed....

Obvious case of using the right technology to rough and then righter (sic) technology to finish machine.

When/if people ask why we do it that way (machine extra holes), we simply say it is part of our process and it doesn't cost them any more or less.

Actually it saves us time and money but its too hard to explain how you actually SAVE money by doing more cutting - albeit with somebody else's laser as opposed to our own CNC.

[InspirationTool]

NC Cams:

Is HR (I assume hot rolled) plate have a low carbon content? I would assume the edges from the laser are glass hard and would give you problems on the mill, but it sounds like it wasn't a problem.

-Jeff

[NC Cams]

HR is hot rolled low carbon steel. The lack of carbon does tend to make it harden or maintain hardness in parts, with or without a quenchant.

When you laser cut, you actually have a problem with DECARBURIZATION at the cut zone - thus the material is more prone to cracking because the stuff has be "fried" so hard.

Moreover, the laser cutting process does NOT involve a quenchant - you generally have to oil or water quench to harden steel (unless it is air hardenable).

Hence, the laser cut zone is not appreciably hard when you're using HR steel. Interestingly, we also did some 4140 parts using the same method - ditto the hardness situation.

By the way, low carb steel is actually a bit uglier to machine because it is so "gummy" and soft - harder, higher carbon steels can actually cut "nicer" as with respect to machine finish.

[Geof]

Originally Posted by InspirationTool NC Cams: Is HR (I assume hot rolled) plate have a low carbon content? I would assume the edges from the laser are glass hard and would give you problems on the mill, but it sounds like it wasn't a problem. -Jeff

With HR steel which is low carbon the edges are going to be negligibly harder than the rest of the material; HR steel simply has insufficient carbon to harden noticeably. You do have a heat affected zone immediately adjacent to the cut but with laser this is very small and the condition of the surface will depend on the gas used in the laser system. Pure Nitrogen will give a very clean surface with no scale; air will give a slightly scaled surface. If you try taking a very shallow cut on this scale with a HSS tool you will have poor tool life. With carbide or as soon as you take the cut in beyond about 20 to 50 thou you are cutting under the affected zone into unaltered material and there should be no problem. Also if you climb cut your cutter does not rub against the surface as it enters the cut.

The situation does not change much even when you are dealing with a medium or high carbon steel or an alloy steel. These steels can be hardened and in the heat affected zone they do harden because the bulk material acts as a heat sink and 'quenches' the heated material either side of the cut. Trying to cut these surfaces with a HSS tool may not be at all successful but provided you have a machine that can take a 50 thou or more depth of cut the full thickness of the material with a feed of several thou per tooth at maybe half the sfm that would be used for unaffected material you should have no problems.

If you do not have a machine that has the capacity to remove the heat affected zone in a single pass; i.e. machine too small or material too thick, then it is a toss up whether you go to abrasive waterjet cut material (more expensive) which has no heat so the cut edge is completely unaltered or just accept shorter tool life on the cutter used for the first passes around the cut edge (higher tool costs).

If you do have a nice big machine and you are putting the required precision into the parts in the mill then the cutting precision may not be so important. It is possible you could get the blanks cut out at lower cost using plasma. This gives a much deeper heat affected zone but in low carbon steel with a good machine it is possible to get it off in one cut. A drawback to plasma is that the fixturing holes you get cut will not look as clean as laser cut so for a nice looking finished product you may have to clean up these. This would probably negate the saving from plasma cutting.