Design for manufacturing - Laser Cutting or Water Jet Cutting technologies

[elinah34]

Hello,

I want to allow the supplier to manufacture (at least contour cutting) the attached sheet metal by Laser Cutting or Water Jet Cutting technologies.
Which type of corners is best for these technologies? Which one is impossible?

Thanks,

 

[Jboggs]

All possible. None impossible. Every cutting method has its own issues as far as edge quality, but since both are based on simple x,y motions, the geometry is feasible.

 

[dgeesaman]

In my experience, you can't get sharp corners from any cutting technique. All cutting tools have an innate cutting width that rounds an internal corner. That is why radii are generally used on inside corners and chamfers or radii are used on outside corners. Mechanically we know radii reduce stress in most internal corners.

I don't think Laser or water jet care a whole lot about how they cut inside corners, especially if the material is thin (say under 1/4"). Laser reaches its thickness limit before water. With waterjet the stream both expands and lags through the thickness but some machines can compensate for that to make dead square cuts. Laserjet applies heat to the part which can be an issue. Finish edge quality is never perfect with any of them.

Flame cutting and plasma cutting are also quite good and I think they're cheaper than jet cutting. Not quite as controlled and accurate but if your contour is suitable it can save money.

Google is your friend if you don't have a vendor willing to talk to you. My company works with a shop that has both laserjet and waterjet so I'm conveniently ignorant of the subtle differences - they take our drawings and choose the best one without our help.

 

[ctopher]

I agree with dgeesaman.
Out of the three images, I would pick the one with fillets. Use standard radii.

 

[elinah34]

In my experience, you can't get sharp corners from any cutting technique. All cutting tools have an innate cutting width that rounds an internal corner. That is why radii are generally used on inside corners and chamfers or radii are used on outside corners. Mechanically we know radii reduce stress in most internal corners.

I don't think Laser or water jet care a whole lot about how they cut inside corners, especially if the material is thin (say under 1/4"). Laser reaches its thickness limit before water. With waterjet the stream both expands and lags through the thickness but some machines can compensate for that to make dead square cuts. Laserjet applies heat to the part which can be an issue. Finish edge quality is never perfect with any of them.

Flame cutting and plasma cutting are also quite good and I think they're cheaper than jet cutting. Not quite as controlled and accurate but if your contour is suitable it can save money.

Google is your friend if you don't have a vendor willing to talk to you. My company works with a shop that has both laserjet and waterjet so I'm conveniently ignorant of the subtle differences - they take our drawings and choose the best one without our help.

So I understand that radii (my preference) are possible. By the way, I think that once there are counterinks the parts will be machined in CNC. I am not sure if cutting by one method and final machining by another method is efficient.

 

[elinah34]

I agree with dgeesaman.
Out of the three images, I would pick the one with fillets. Use standard radii.

Thanks

 

[dgeesaman]

So I understand that radii (my preference) are possible. By the way, I think that once there are counterinks the parts will be machined in CNC. I am not sure if cutting by one method and final machining by another method is efficient.

You almost always have to start with a cutting process on a piece of raw material. Then if machining is necessary, that happens afterward.

The cheapest designs always maximize the use of the cutting process and minimizes or eliminates machining.

Countersunk holes are a bear because they always put shear stress on the bolt when there are more than one in a bolted joint. They require very tight positional tolerances and assembly requires great care. Use standard through holes as much as possible, then counterbored holes, and countersunk as a last resort.

 

[elinah34]

You almost always have to start with a cutting process on a piece of raw material. Then if machining is necessary, that happens afterward.

The cheapest designs always maximize the use of the cutting process and minimizes or eliminates machining.

Countersunk holes are a bear because they always put shear stress on the bolt when there are more than one in a bolted joint. They require very tight positional tolerances and assembly requires great care. Use standard through holes as much as possible, then counterbored holes, and countersunk as a last resort.

Thanks...I understand, but the bolt mustn't protrude, and a counterbore for M5 bolt that doesn't have conical head requires a thick plate (now it's about 4 mm). Any suggestions?

 

[MintJulep]

To make a sharp corner the machine head must decelerate and come to a complete stop in one axis, then accelerate to speed in a different direction. That takes time, and during that time the power input per unit path length either changes, or the machine needs (try) to compensate for it. That means the cut surface changes approaching and leaving the corner.

For a curved path like a fillet the machine head motion can change smoothly in two axes and the path speed and power per unit length can remain constant. This results in a smoother, more consistent cut.

A chamfer is somewhere in between.

A 5-axis machine can cut countersinks or other features that are not orthogonal to the material surface. That's not to say it's a desirable way to make countersinks for small fasteners.

 

[elinah34]

To make a sharp corner the machine head must decelerate and come to a complete stop in one axis, then accelerate to speed in a different direction. That takes time, and during that time the power input per unit path length either changes, or the machine needs (try) to compensate for it. That means the cut surface changes approaching and leaving the corner.

For a curved path like a fillet the machine head motion can change smoothly in two axes and the path speed and power per unit length can remain constant. This results in a smoother, more consistent cut.

A chamfer is somewhere in between.

A 5-axis machine can cut countersinks or other features that are not orthogonal to the material surface. That's not to say it's a desirable way to make countersinks for small fasteners.

thanks!

 

[BrianPetersen]

Use rounded corners for the reason that MintJulep explained very well.

Cutting followed by CNC is common, but make sure you have good datum surfaces to locate the part in the CNC fixture. The kerf width is non-zero and needs to be accounted for. Any positioning error (or error in kerf width correction) will result in your countersinks being off-center on the holes. Maybe that matters, maybe it doesn't, we don't know what you're using this part for. If it's critical, it's tempting to waterjet the outside shape and CNC all the holes.

 

[dgeesaman]

Thanks...I understand, but the bolt mustn't protrude, and a counterbore for M5 bolt that doesn't have conical head requires a thick plate (now it's about 4 mm). Any suggestions?

Clearance hole in the mating part threading into a nut on the far side. Then each screw will center on the countersink feature. If you must mate to a single part with tapped holes you will simply have to tolerance tightly enough to avoid the fit-up problems.

 

[Jboggs]

OP,
Look at the option of LOW HEAD socket head cap screws. I have used them in many applications. They eliminate the need for countersunk screws, which ALWAYS cause problems. From McMaster:

 

[ctopher]

From the image, and the use of laser cutting, my guess it's a thin part. C'Sink may be the only way to go for this part?

 

[elinah34]

Use rounded corners for the reason that MintJulep explained very well.

Cutting followed by CNC is common, but make sure you have good datum surfaces to locate the part in the CNC fixture. The kerf width is non-zero and needs to be accounted for. Any positioning error (or error in kerf width correction) will result in your countersinks being off-center on the holes. Maybe that matters, maybe it doesn't, we don't know what you're using this part for. If it's critical, it's tempting to waterjet the outside shape and CNC all the holes.

I guess you don't determine how the part will be manufactured, but the required tolerances and the manufacturer decision based on it.

 

[elinah34]

From the image, and the use of laser cutting, my guess it's a thin part. C'Sink may be the only way to go for this part?

Its thickness is 5 mm

 

[BrianPetersen]

I guess you don't determine how the part will be manufactured, but the required tolerances and the manufacturer decision based on it.

I don't understand this sentence.

In the theoretical world, the drawing doesn't dictate the manufacturing process, it just identifies the critical features of the part and the relevant dimensions and tolerances, and it's up to manufacturing to figure it out. You do the drawing, you toss it over the wall, manufacturing department builds it ... sometimes with a whole bunch of cussing and swearing that could have been avoided.

In the real world, if you design a part that can't be easily manufactured for whatever reason, you are either going to pay a lot more than you otherwise would in order for a fabricator to jump through hoops when there could have been an easier way had certain design choices been made, or you are going to have an angry shop foreman coming to see you because they can't do what you're asking them to do, or some combination.

The smart designer has a little discussion with the fabricator when there's a question about how best to design something so that it can be as easy as possible to make while still performing its intended function, so even though the eventual drawing doesn't dictate the manufacturing process, the features and dimensions lead to a logical process for making it.

With both waterjet and laser (and plasma), there's tradeoffs between how fast, how accurate, how good the surface finish will be, and how much power your machine has.

 

[DAVIDSTECKER]

Years ago, when having parts laser cut, even with low carbon 1018/1020, there is a heat effected zone that is very hard.
It was a big problem when we tried to tap the holes.
I ended up using a 1008 steel.

 

[elinah34]

Years ago, when having parts laser cut, even with low carbon 1018/1020, there is a heat effected zone that is very hard.
It was a big problem when we tried to tap the holes.
I ended up using a 1008 steel.

What about aluminum?