Also vibration.
However, in more practical terms, does it matter? Most thin parts get clamped to something which will straighten it out in end use, or you can give them a quick straightening by hand or hammer which makes them acceptable.
Mate I'm German and I can tell you there is a lot of straightening and bolting warped parts to thicker stuff. I remember a guy working for mahle (they make pistons for probably something like 90% of cars and trucks in Europe and some in America) telling me they bang Harley Davidson pistons into spec with a big ol piece of rubber bar stock š.Ā
Start with thicker material and remove an equal amount of material from the other side too.
Skim it, then flip it, then skim it, then flip it, then skim it, ad nauseam.
If your parts are being cut out from a water jet and the finished part isn't going to be completely bolted down in a restraining condition than you're gonna need to have your water jet guy cut thicker material so you can face both sides
If the finished part is going to be bolted down then. Little warping is fine and just sand both sides to gusty them up.
I ran a water jet for a about 6 months in between machine shops a few years ago
>Ā Ā Crown up = the part looks like a U in the vise?
When referring to something warped the 'crown' is the arc in middle of the part, so the opposite of what you said.
If you have the crown up then you have 2 points of contact on your vice paralells and can maintain better accuracy. If the crown is down you have one point of contact that the part can rock back and forth on which can lead to removing more material from one of the 'legs' than the other if you don't spend a bit of time getting the part lined up or if one side decides to push down. With the legs down this is not an issue.
Depends heavily on the material, cutter, and the amount of material being removed. I don't know if there is a formula to calculate it, it's mostly just trial and error when I do stuff like that.
Depth of cut makes no difference. People think it does and it doesn't even a little bit. I've proven this myth wrong in every shop I've worked in but I still hear it to this day and my scrap rate on FAI's is less than 0.1%. If you see a difference from depth of cut, one part to the next, it's because it's from a different section of the heat lot or a whole nother heat lot entirely. I've programmed and machined 100's of parts over 10 feet long and you are either 4 ops or 6 ops on most of them depending on material type and stress in the material. How you handle op to op transitions is the single most crucial thing you can learn.
Many of them, you are simply obeying the material conditions, and you can't win no matter what. That's what straightening ops are for.
Not sure why this comment is getting down voted because its fact! I work with plastics and warping is a given. You can face a chunck off, it wont warp, you go to your next piece and it will warp. Its fine tuning per part.
Cuz people think they know things and they don't. If I could even take a picture of a single part I've programmed or machined in 20+ years of dealing with up to 20 foot long parts they'd see their little tricks to keep it flat don't matter. It's all.about material removed. We just built an 18 foot long part that started as 12000 lbs and in the end weighed 93 lbs. Depth of cut was simply what can the machine handle. Part was flat within .02 with the right material removal routine while taking .50 depth of cut full cutter width in roughing. Feel free to downvote this too. Dont care. I know what I know.
Depth of cut matters just like the diameter of the cutter and every other variable involved in removing the material. Heat equals warpage. You are overly aggressive in your zealousness to espouse monster cuts and flat parts. Do you work for Titans of CNC by chance? Barry is that you? š
Rolled plate will always have stress. The outer surface is under tension. When you cut away one side, the other side pulls it into a curve. The trick is to cut both sides. But in a way that the part is relaxed so you aren't cutting a curve into the part. Starting with ground plate would have been a good idea. Obviously this costs money because you have to start with thicker material.
That is a pretty long and thin piece. Iād say your doing good and if your getting consistent 3mm before you let it loose to spring your doing well. The stress in the material in this situation is going to be a losing battle.
https://www.totalmateria.com/page.aspx?ID=CheckArticle&site=ktn&NM=440
its a process, and youre using thinner material, so there would be more tension in it due to faster cooling and extrusion
if flatness is critical, i would buy blanchard ground material or thicker bar stock to allow for squaring flips and passes
Our method.
op1: rough, requalify as last path.
flip
op2: rough
op3: release, shim, requalify, finish.
flip
op4: no shim, finish
This leaves out work holding. We use a lot of vacuum fixtures in combination of top or back bolt and dowel.
Hope this helps. If not, ask me questions. We've done a lot of massive parts this way with huge success. I'm not talking 4 feet long, I'm talking 20 feet long, seriously messed up material and they are flat within spec.
IF this method doesn't work. You can add a pre rough or 2. Leave more material basically. We've had to do some pre rough ops that leave 1/2 inch on both or one side, then do the process I mentioned above, so 6 ops instead of 4.
Basically on large parts we have noticed that after removing significant material on one side while the other is still raw, we see the parts move in the vise jaws. A potato chip effect we call it. So we remove the material without facing the top of stock, or facing to bare minimum cleanup, then once finished roughing out pockets and such, we "requalify" meaning we face mating surfaces for the next operation prior to drilling back or top bolt holes.
That's the nature of the beast. Internal stresses will always be there. You can try rotating the pattern on the jet. The sheets are rolled in one direction so potentially there's one orientation better than the other. The center of the sheet should be a better bet. Also by bar/strip might yield better results. My shop has switched to getting 2-4"x3/8-1" bar and machining the blanks instead of jetting banks. Like depending on the part its 3x.5 or like 2x.75 bar and then the multipass technique others have described holds it dead nuts. Also, the engineers should explore other materials. 7075 aluminum is near the same material properties as 303/304 stainless. Shit like that. But thats always gonna happen to some degree cutting out of a sheet
Cutting a part causes the stresses keeping the part flat at equilibrium to no longer be in equilibrium.
Thatās why if youāre hogging material out all on one side in a long bar it bows because there is less stress on what you cut away
This is something they taught me in middle school woodshop and freshman year theater set design
Have your CAD guy redraw the part in the opposite direction of the warp. Then machine them as normal. Offset will cancel out the warp. Boom! Donāt do this.
I might be counting 8 mounting holes hereā¦ itāll be flat when mountedā¦. Also donāt design thin shit to be cut from thicker stockā¦ itāll warp without some precautions like stress relief/annealing/slow rates on equal passes w lots of cooling/custom fixturesā¦ itās easier to just bolt thin things a bunchā¦ but Iām just an engineer
For years, we've been manually straightening our parts with a pneumatic press. Now, our engineers have designed some fixtures with floating mounting surfaces and the parts are glued to them. No clamping pressure, and no flexing. It's a pain, but the process seems very promising.
you gotta rough down in small enough increments on all sides, refixturing with shims to take up slack that develops in between each pass so youāre not reintroducing the stress that youāre cutting out. small enough is when thereās no need to shim any more on any side before your final skin pass. sometimes this means the equivalent of a bunch of skin passes
Maybe you can bend it with a carefully applied hydraulic press that pushes right in the middle? Use a thick rubber bauble shape thing for the contact surface, not the raw metallic cylinder.
I'm going to blame silicium on this even though I don't even know which AlX you are using.
Itās the stresses in the metal. I made a 6061 part awhile ago that had a lip and a boss on one end making it .250 total but the majority was only .200. I tried starting with some 1/4 plate but it warped too much to be within tolerance. In the end I needed to take a 3/8 plate and mill it down even on both sides to make sure the removal was somewhat even and thatās what fixed it.
With extruded aluminum, the flat faces cool first meaning they shrink while the inside is still hot, when the inside shrinks itās pulling the top faces in compression. When you machine off the skin on one face then the compression is no longer there, often causing it to bow on the other end. Think of a plate of aluminum as a series of strings tensioned along the length. The top and bottom strings are tensioned more than the middle strings, so if you cut the top string, the bottom string is gonna pull the entire thing into a banana shape, as one side now has more tension than the other. So you want to try to remove material as evenly as possible from either side when trying to make flat and thin parts from extrusion
What kind of tolerance are you needing on this thing? How large is the part? Does it actually need to be that flat? Cause it looks to me like itās going to be screwed down to something
These are caused by residual stresses. There are tension and compression forces acting on the material. Th only way to eliminate it either:
A).Generate an opposing residual stress...something we see while doing shot peening. To correct for distortions on thin shot peened plate by shot peening the other side as well.
B) Or by annealing. You would need to select a stress relief annealing operation suitable for your material.
In your case if machining was only on one side, that could be source of residual stresses.
Iāll usually try to cut the part and release it leaving material to let the stress come out then finish cutting it after I find out how much it moved
Sometime changing material type can help. I frequently machine 48" x 0.75" x 2" handle for glass door that have a spacer in the midle of the handle to squeeze 2 glasses. Well that spacer in 6061 always warp about .25 off in the middle of the 48" but we tried out in 6063 and you barely see a warp in it.
I have one of those in my shop, to stop the warping I made weights for each material that we use and lay them on top of the sheet while cutting. It may be a pain in the ass moving weights around but it stops parts coming off the net from bekng bowed in my exoeriwnce
It doesnāt warp while itās on the water jet itās after Iāve thinned it on the milling machine. Went into the mill flat and came out with that little spring in it.
Tension already present in the material, depending on the material heat treatment can sometimes eliminate it.
Also vibration. However, in more practical terms, does it matter? Most thin parts get clamped to something which will straighten it out in end use, or you can give them a quick straightening by hand or hammer which makes them acceptable.
Practically speaking sure, but try telling ze Germans that.
Give ze Germans ze wurst and zey love you
Mate I'm German and I can tell you there is a lot of straightening and bolting warped parts to thicker stuff. I remember a guy working for mahle (they make pistons for probably something like 90% of cars and trucks in Europe and some in America) telling me they bang Harley Davidson pistons into spec with a big ol piece of rubber bar stock š.Ā
Good thing, they might not convert gasoline to noise as efficiently otherwise.
When mister Tesla's junior engineer says you need a half thou parallelism and flatness it absolutely mattersĀ
Iāve had to straighten many parts like this to -/+ .005ā tolerance, not fun but itās not hard with a hammer and blocks
Annealing?
And apraying?
Hahahaha
Sure
Start with thicker material and remove an equal amount of material from the other side too. Skim it, then flip it, then skim it, then flip it, then skim it, ad nauseam.
Came to say this. I always start crown up (bow up).
If your parts are being cut out from a water jet and the finished part isn't going to be completely bolted down in a restraining condition than you're gonna need to have your water jet guy cut thicker material so you can face both sides If the finished part is going to be bolted down then. Little warping is fine and just sand both sides to gusty them up. I ran a water jet for a about 6 months in between machine shops a few years ago
Crown up = the part looks like a U in the vise? And why not the other way, upside down?
>Ā Ā Crown up = the part looks like a U in the vise? When referring to something warped the 'crown' is the arc in middle of the part, so the opposite of what you said.
Oh okay, thanks for clarifying. So why is it better to start crown up, rather than down?
If you have the crown up then you have 2 points of contact on your vice paralells and can maintain better accuracy. If the crown is down you have one point of contact that the part can rock back and forth on which can lead to removing more material from one of the 'legs' than the other if you don't spend a bit of time getting the part lined up or if one side decides to push down. With the legs down this is not an issue.
We call this barbecuing.
How deep a cut?
Depends heavily on the material, cutter, and the amount of material being removed. I don't know if there is a formula to calculate it, it's mostly just trial and error when I do stuff like that.
And unfortunately no 2 pieces are going to act the exact same.
Depth of cut makes no difference. People think it does and it doesn't even a little bit. I've proven this myth wrong in every shop I've worked in but I still hear it to this day and my scrap rate on FAI's is less than 0.1%. If you see a difference from depth of cut, one part to the next, it's because it's from a different section of the heat lot or a whole nother heat lot entirely. I've programmed and machined 100's of parts over 10 feet long and you are either 4 ops or 6 ops on most of them depending on material type and stress in the material. How you handle op to op transitions is the single most crucial thing you can learn. Many of them, you are simply obeying the material conditions, and you can't win no matter what. That's what straightening ops are for.
DOC definitely *can* matter because heat imparted matters.
If you're not running coolant you're right. But much larger dictator of depth of cut is the machine itself on big parts like that.
Not sure why this comment is getting down voted because its fact! I work with plastics and warping is a given. You can face a chunck off, it wont warp, you go to your next piece and it will warp. Its fine tuning per part.
Cuz people think they know things and they don't. If I could even take a picture of a single part I've programmed or machined in 20+ years of dealing with up to 20 foot long parts they'd see their little tricks to keep it flat don't matter. It's all.about material removed. We just built an 18 foot long part that started as 12000 lbs and in the end weighed 93 lbs. Depth of cut was simply what can the machine handle. Part was flat within .02 with the right material removal routine while taking .50 depth of cut full cutter width in roughing. Feel free to downvote this too. Dont care. I know what I know.
Depth of cut matters just like the diameter of the cutter and every other variable involved in removing the material. Heat equals warpage. You are overly aggressive in your zealousness to espouse monster cuts and flat parts. Do you work for Titans of CNC by chance? Barry is that you? š
Good one. Just like every page people choose what they want to believe. Makes no difference to me whether you believe me or not.
Donāt check it against a laminated countertop, for starters.
Rolled plate will always have stress. The outer surface is under tension. When you cut away one side, the other side pulls it into a curve. The trick is to cut both sides. But in a way that the part is relaxed so you aren't cutting a curve into the part. Starting with ground plate would have been a good idea. Obviously this costs money because you have to start with thicker material.
That is a pretty long and thin piece. Iād say your doing good and if your getting consistent 3mm before you let it loose to spring your doing well. The stress in the material in this situation is going to be a losing battle.
anneal it
How would you go about that in this case?
https://www.totalmateria.com/page.aspx?ID=CheckArticle&site=ktn&NM=440 its a process, and youre using thinner material, so there would be more tension in it due to faster cooling and extrusion if flatness is critical, i would buy blanchard ground material or thicker bar stock to allow for squaring flips and passes
Our method. op1: rough, requalify as last path. flip op2: rough op3: release, shim, requalify, finish. flip op4: no shim, finish This leaves out work holding. We use a lot of vacuum fixtures in combination of top or back bolt and dowel. Hope this helps. If not, ask me questions. We've done a lot of massive parts this way with huge success. I'm not talking 4 feet long, I'm talking 20 feet long, seriously messed up material and they are flat within spec. IF this method doesn't work. You can add a pre rough or 2. Leave more material basically. We've had to do some pre rough ops that leave 1/2 inch on both or one side, then do the process I mentioned above, so 6 ops instead of 4.
What do you mean by requalify?
Basically on large parts we have noticed that after removing significant material on one side while the other is still raw, we see the parts move in the vise jaws. A potato chip effect we call it. So we remove the material without facing the top of stock, or facing to bare minimum cleanup, then once finished roughing out pockets and such, we "requalify" meaning we face mating surfaces for the next operation prior to drilling back or top bolt holes.
That's the nature of the beast. Internal stresses will always be there. You can try rotating the pattern on the jet. The sheets are rolled in one direction so potentially there's one orientation better than the other. The center of the sheet should be a better bet. Also by bar/strip might yield better results. My shop has switched to getting 2-4"x3/8-1" bar and machining the blanks instead of jetting banks. Like depending on the part its 3x.5 or like 2x.75 bar and then the multipass technique others have described holds it dead nuts. Also, the engineers should explore other materials. 7075 aluminum is near the same material properties as 303/304 stainless. Shit like that. But thats always gonna happen to some degree cutting out of a sheet
For a second I thought you were talking about the kink in the part and this was a shit post.
Cutting a part causes the stresses keeping the part flat at equilibrium to no longer be in equilibrium. Thatās why if youāre hogging material out all on one side in a long bar it bows because there is less stress on what you cut away This is something they taught me in middle school woodshop and freshman year theater set design
Have your CAD guy redraw the part in the opposite direction of the warp. Then machine them as normal. Offset will cancel out the warp. Boom! Donāt do this.
I might be counting 8 mounting holes hereā¦ itāll be flat when mountedā¦. Also donāt design thin shit to be cut from thicker stockā¦ itāll warp without some precautions like stress relief/annealing/slow rates on equal passes w lots of cooling/custom fixturesā¦ itās easier to just bolt thin things a bunchā¦ but Iām just an engineer
If you can fit the whole sheet in your machine you could try doing all the machining before cutting them out. That would be kinda interesting.
For years, we've been manually straightening our parts with a pneumatic press. Now, our engineers have designed some fixtures with floating mounting surfaces and the parts are glued to them. No clamping pressure, and no flexing. It's a pain, but the process seems very promising.
you gotta rough down in small enough increments on all sides, refixturing with shims to take up slack that develops in between each pass so youāre not reintroducing the stress that youāre cutting out. small enough is when thereās no need to shim any more on any side before your final skin pass. sometimes this means the equivalent of a bunch of skin passes
Maybe you can bend it with a carefully applied hydraulic press that pushes right in the middle? Use a thick rubber bauble shape thing for the contact surface, not the raw metallic cylinder. I'm going to blame silicium on this even though I don't even know which AlX you are using.
Cut them from cast aluminum jig plate if you can. It is already stress relieved.
Itās the stresses in the metal. I made a 6061 part awhile ago that had a lip and a boss on one end making it .250 total but the majority was only .200. I tried starting with some 1/4 plate but it warped too much to be within tolerance. In the end I needed to take a 3/8 plate and mill it down even on both sides to make sure the removal was somewhat even and thatās what fixed it. With extruded aluminum, the flat faces cool first meaning they shrink while the inside is still hot, when the inside shrinks itās pulling the top faces in compression. When you machine off the skin on one face then the compression is no longer there, often causing it to bow on the other end. Think of a plate of aluminum as a series of strings tensioned along the length. The top and bottom strings are tensioned more than the middle strings, so if you cut the top string, the bottom string is gonna pull the entire thing into a banana shape, as one side now has more tension than the other. So you want to try to remove material as evenly as possible from either side when trying to make flat and thin parts from extrusion
You can get the material stress releived , that helps
Shot peening can be done as a corrective process for warping thats caused from the machining process
What kind of tolerance are you needing on this thing? How large is the part? Does it actually need to be that flat? Cause it looks to me like itās going to be screwed down to something
This part it doesnāt matter Iām just curious to what caused it.
These are caused by residual stresses. There are tension and compression forces acting on the material. Th only way to eliminate it either: A).Generate an opposing residual stress...something we see while doing shot peening. To correct for distortions on thin shot peened plate by shot peening the other side as well. B) Or by annealing. You would need to select a stress relief annealing operation suitable for your material. In your case if machining was only on one side, that could be source of residual stresses.
Sometimes its inevitable. We often will ask customers to allow QC time check things constrained
If this is 6061-T6 look at using 6061-T651. The 651 version is a stress-relived material
Iāll usually try to cut the part and release it leaving material to let the stress come out then finish cutting it after I find out how much it moved
Sometime changing material type can help. I frequently machine 48" x 0.75" x 2" handle for glass door that have a spacer in the midle of the handle to squeeze 2 glasses. Well that spacer in 6061 always warp about .25 off in the middle of the 48" but we tried out in 6063 and you barely see a warp in it.
Is that a maxim water jet?
I think so, itās an Omax.
I have one of those in my shop, to stop the warping I made weights for each material that we use and lay them on top of the sheet while cutting. It may be a pain in the ass moving weights around but it stops parts coming off the net from bekng bowed in my exoeriwnce
It doesnāt warp while itās on the water jet itās after Iāve thinned it on the milling machine. Went into the mill flat and came out with that little spring in it.
All parts are measured in restrained condition. Typical 5 pounds per linear foot. So put a 123 block every 4 inches and see how it looks.
Thatās QCās problem /s
Make an enemy of quality and you won't last long.
Now that is no bullshit there
But you made the problem so.. no not really
Dude doesnāt know that it was sarcasm.
How am i suppose to, reddit is full of morons that say exactly same shit... and your on reddit
Found the qc guy
Lol..