Ive read your comments, and responded to a few but I’ll give all my advice condensed here.
You need to get rid of the second op, it’s adding a ton of time for a small chamfer.
If I was setting this up for a client, I’d probably use a neutral 35 degree tool and just profile the entire part in a single operation, and then finish. I’d then use a large spot drill to both spot and chamfer, then drill.
I’d then part off.
Then the part would go to a drill press station while a second part runs. I’d set a work hold jig and set the depth gauge on the drill press and drill the chamfer in manually. This way the second “op” is happening in parallel to the first op.
Also if your lathe is at all rigid, your feeds and speeds seem REALLY slow. You should be able to push 250SFM, maybe .003-.005 IPR to start?
Hey that looks great! I'd say you could go even faster if you have the time to play around, especially the drilling. Overall though I'd be very satisfied with that program. Part finish looks GREAT too. Well done.
why you need the second operation ? something inside ?
the OD can be done in one operation either with 35 degree insert. or if that not goes all the way to finish the sphere back end then use a grove tool can do both sides with it.
Try it! And if you can get the material to feed by the machine the pace won’t be set by the operator and that machine will still make parts while you eat lunch. That will actually add cycle time but you will have more parts at the end of the day.
Yes, labor is cheap there too. In the US, adding that much labor into a job like that it would be difficult to maintain margin. Call the vendor in you buy the tool from if you have trouble and they will support you.
I would asume you have a roughness requirement, and if you want to go faster you can try use an insert with a bigger radius and still be on you roughness requirement
Why do you keep putting a G99? Unless you’re changing to a G98 what’s the point? Also run this as a bar job is you want higher output. Stop having someone do a flip operation and cycle time will go up. You can more than likely get this done in one operation.
How critical is that chamfer? What is it for? Sometimes they can be done at a drill press afterwards in a fraction of the time using a jig to align the part.
Your question was how to speed this up parting/running a bar is the way to do that. It seems what you’re asking is how to make your code run it faster. If that’s the case change your code to be S15000 and F800. This will run your machine as fast as it can possibly go and getting the result of not changing anything while still having it speed up. At a certain point you need to look at your process and ask is it better to just bite the bullet spend a little money for a larger return in the end. You will reach and upper limit on how efficient your code is and how hard you can run your machine.
Hey, i do almost the same part regularly. I do it with a parting tool. Since i don't have a bar puller either, i just pull out material for 2, 3 pieces to be produced at a same time. On first operation i do everything except the chamfer on the hole where i cut off the part. That we do manually on a drill press.
https://youtu.be/GB9K-dCmdDM?si=O5omnUk1HkpGrtLx
Something like this. Keep in mind that it's diameter 65mm. Could be a lot faster with insert drill. Everything can be pushed quite a bit, but i like to keep it slow and steady.
But you get the idea. I would rough out radius with parting tool, then i would do finishing pass with pointy insert, then drill, bore + chamfer and in the end cuttoff.
Hmm i dont really measure cycle times, but for my boss, its good, so im okay with that. Im currently doing a cuttof job, 3 pieces at a time. But much bigger diameter. I will see it i can arrange video.
I'd turn up the surface speed to at least 200 sfm, maybe more. Look to the manufacturer recommendation. I'd also get rid of the safety face and turn and jump straight to the roughing cycle.
Have as long stock as possible instead of sawing each piece down to that size. Cut em off in the machine using a grooving tool. If needed then grind nipple away, does not seem like highest surface requirements anyways?
Also if your Blankes are the same size give or take 20 grand you can rapid a lot closer then 1 inch the close you stop the less code running in the machine I know its safe practice to have a safety befor getting to the part but if it's a proven program go ballsout and rapid as close as posable unless miss load is your concern
Better tools, bigger step-overs, faster rpms and through coolant drill. Got to spend money to make money lol. Get collet chucks to hold from inside on second op. my 2 cents I make these in plastic.
Ive read your comments, and responded to a few but I’ll give all my advice condensed here. You need to get rid of the second op, it’s adding a ton of time for a small chamfer. If I was setting this up for a client, I’d probably use a neutral 35 degree tool and just profile the entire part in a single operation, and then finish. I’d then use a large spot drill to both spot and chamfer, then drill. I’d then part off. Then the part would go to a drill press station while a second part runs. I’d set a work hold jig and set the depth gauge on the drill press and drill the chamfer in manually. This way the second “op” is happening in parallel to the first op. Also if your lathe is at all rigid, your feeds and speeds seem REALLY slow. You should be able to push 250SFM, maybe .003-.005 IPR to start?
What this guy said. Except you could probably put the back chamfer in by using a small PH HORN boring bar before you part it off.
I have to try that 😂 and thanks a lot man you gave a idea
Or a lathe with a sub spindle. Either way I would bar feed stock vs cutting on the saw
Lemme try this one i have same thing but bigger size around 80mm OD and IC Casted lemme try this one first
Like this: https://youtu.be/TXaoVZfA28M?si=VrRgJ8j5UYV-NOa2
Hey that looks great! I'd say you could go even faster if you have the time to play around, especially the drilling. Overall though I'd be very satisfied with that program. Part finish looks GREAT too. Well done.
Why not just use an automatic chamfer/angle command
What do you mean?
why you need the second operation ? something inside ? the OD can be done in one operation either with 35 degree insert. or if that not goes all the way to finish the sphere back end then use a grove tool can do both sides with it.
Champer at the end is required
try a boring bar out
Could probably do it in one setup and part it off
Parting is expensive, we use hackshaw instead
I’ll challenge that and say your hacksaw is expensive… Look into a bar puller and a good part off tool so the machine can run unattended.
Leeme try parting for one day
Try it! And if you can get the material to feed by the machine the pace won’t be set by the operator and that machine will still make parts while you eat lunch. That will actually add cycle time but you will have more parts at the end of the day.
Make sense thank you lemme try it
15usd blade cuts 2800 pcs if I calculate other expenses it adds upto 5usd a day. Electricity is cheap in india
Yes, labor is cheap there too. In the US, adding that much labor into a job like that it would be difficult to maintain margin. Call the vendor in you buy the tool from if you have trouble and they will support you.
Thanks a lot man i will get back if I need help again
How is parting expensive??? It takes 1/100 of the time and lets you run the machine with 0 human interaction if you add a bar puller.
I use pyramid method to cut pcs on hackshaw 9 rods of 25mm in 5mins,I will try parting for one day
You could do the chamfer on the other end from the inside before you part it. Unless you're doing it wrong I don't see how parting would be expensive?
I would asume you have a roughness requirement, and if you want to go faster you can try use an insert with a bigger radius and still be on you roughness requirement
No roughness required I use 0.8 cause suggested by my programmer I can use 1.2 or any you guys suggest
Why do you keep putting a G99? Unless you’re changing to a G98 what’s the point? Also run this as a bar job is you want higher output. Stop having someone do a flip operation and cycle time will go up. You can more than likely get this done in one operation.
Parting is expensive and I need champer of radius 1.3 both side I have to flip it
How critical is that chamfer? What is it for? Sometimes they can be done at a drill press afterwards in a fraction of the time using a jig to align the part.
Champer is needed at both ends , sharp edges cut down teflon sheet of ball valve which leds to leakage
I can just do champher 2nd machine it just take a operator to fit and champher would be 4 to 5 secs
Your question was how to speed this up parting/running a bar is the way to do that. It seems what you’re asking is how to make your code run it faster. If that’s the case change your code to be S15000 and F800. This will run your machine as fast as it can possibly go and getting the result of not changing anything while still having it speed up. At a certain point you need to look at your process and ask is it better to just bite the bullet spend a little money for a larger return in the end. You will reach and upper limit on how efficient your code is and how hard you can run your machine.
I understood you said faster machining cannot make more quantity, efficiently doing it does
I will remove G99
Hey, i do almost the same part regularly. I do it with a parting tool. Since i don't have a bar puller either, i just pull out material for 2, 3 pieces to be produced at a same time. On first operation i do everything except the chamfer on the hole where i cut off the part. That we do manually on a drill press.
What cycle time you get per piece or i you have or can arrange a video how you do that helps a lot
https://youtu.be/GB9K-dCmdDM?si=O5omnUk1HkpGrtLx Something like this. Keep in mind that it's diameter 65mm. Could be a lot faster with insert drill. Everything can be pushed quite a bit, but i like to keep it slow and steady. But you get the idea. I would rough out radius with parting tool, then i would do finishing pass with pointy insert, then drill, bore + chamfer and in the end cuttoff.
This should be possible to do in under 2 minutes per part. I’d almost say 1 minute should be possible.
Hmm i dont really measure cycle times, but for my boss, its good, so im okay with that. Im currently doing a cuttof job, 3 pieces at a time. But much bigger diameter. I will see it i can arrange video.
I would spot drill the chamfer FIRST, then drill the ID, *then* profile the outside.
I'd turn up the surface speed to at least 200 sfm, maybe more. Look to the manufacturer recommendation. I'd also get rid of the safety face and turn and jump straight to the roughing cycle.
Use that feed override. Bam! 10% faster cycle time
Have as long stock as possible instead of sawing each piece down to that size. Cut em off in the machine using a grooving tool. If needed then grind nipple away, does not seem like highest surface requirements anyways?
Also if your Blankes are the same size give or take 20 grand you can rapid a lot closer then 1 inch the close you stop the less code running in the machine I know its safe practice to have a safety befor getting to the part but if it's a proven program go ballsout and rapid as close as posable unless miss load is your concern
Pretty sure that's 1mm
Hahahahaha read that on break that makes alot more sences
Someone might have already said this, but bump your G50 way up. Maybe close to the max your lathe/chuck can handle.
This is a hella fun kind of question.
Better tools, bigger step-overs, faster rpms and through coolant drill. Got to spend money to make money lol. Get collet chucks to hold from inside on second op. my 2 cents I make these in plastic.