Question for tool and die guys

[maestro]

I have been presented with a draw die assembly for programming. I will start off by saying I have never really done much tool and die work in my career. The female part off the die is a curved cavity 3.4 deep with a .125 fillet radius in the bottom of it. I have attached a pic of this area. We only have 3 axis 40 taper vmc's available for this. My Question to you guys is, will it be feasible to finish this area with a .250 ball nose 3.4 deep without it pushing off too much. To me it seems this area my be better suited for an EDM operation. The gap between the 2 parts of the die is only .016.

[guitar]

You are correct. EDM. Yeah, By the time you mill it, troubleshoot it, pay for the cutters, and then polish it, your edm guy could already have the part to the customer, and actually made money. I am a tool and die guy also.

I am also:

Mold maker

Rotary cut die maker

Indexer maker

barrel cam maker

Auto detailer

pipe fitter

Demolitions tech

landskaper

janitor

computer repair man

burn/laser/punch machine programmer

carpenter

An all around great guy that you would love to know.

 

[Thee Rickster ™]

You are correct. EDM. Yeah, By the time you mill it, troubleshoot it, pay for the cutters, and then polish it, your edm guy could already have the part to the customer, and actually made money. I am a tool and die guy also.

I am also:

Mold maker

Rotary cut die maker

Indexer maker

barrel cam maker

Auto detailer

pipe fitter

Demolitions tech

landskaper

janitor

computer repair man

burn/laser/punch machine programmer

carpenter

An all around great guy that you would love to know.

 

 

Which ones do have certificates for?

[crazy^millman]

What is your draft angle? Can your purchase a die cutter to cut it? Time you OptiCore it, then come back and finish it might be feasible really comes done to do you have the machines to hold the tolerance needed? CAT50 or HSK-100 would be better choice or even a 5 axis machine, but you got what you got and if you approach the toolpaths correctly might still be okay. Are you planning on machining this before or after HT and have you machined hardened metals before? What type of tool steel are you machining? If you need to machine 3.4" deep to a straight wall then makes it very difficult, but not impossible. You mention EDM, but did not say you have that ability on site. If you do then machine what you can leave material for the burn and then go from there. If not then need to consider the lead time, promised delivery and if you have capacity to take the time to machine this in house. If not then farm it out if the price, delivery and expected quality are what you need to get the job done. Without seeing and having something to analyze hard for me to say which is the better way so with that limited information I can say flip a coin.

 

I have been doing this for more than one year so that probably means nothing right guitar? :unworthy: :unworthy:

[Newbeeee™]

You are correct. EDM. Yeah, By the time you mill it, troubleshoot it, pay for the cutters, and then polish it, your edm guy could already have the part to the customer, and actually made money. I am a tool and die guy also.

I am also:

Mold maker

Rotary cut die maker

Indexer maker

barrel cam maker

Auto detailer

pipe fitter

Demolitions tech

landskaper

janitor

computer repair man

burn/laser/punch machine programmer

carpenter

An all around great guy that you would love to know.

 

Hahaha.

Your still FOS.

[Zoober]

Guys a legend....

 

 

 

 

....In his own mind!

[betts]

^^^^ Sure the above. Back to real business, yes you need to answer or address Ron's questions. Many variables but in a shoot from the hip manner I will tell you if I had the ability to do it "in house" and not have to send it to a sinker I would do that. I have finished hard steel in a Fadal that was in need of a tune up and still got the job done. Would you want to do that in a production scenario? No but that is the point of you asking the question.

 

If you have enough draft from your draw angle I would really look at OSG and others who offer "profile" tools that would be for instance a 1/4" ball but have a 3/8" shank with a taper. That principle is available from several manufacturers. So the "pushing off" is relative to how you have roughed it. Don't try to send in a 1/4" ball to finish after a 3/4" bull W/.125R has been the smallest tool in there. There have been times in the past when I have roughed with a 3/8"Ø tool even though I would finish with a 1/2" tool so I didn't bury the finish tool.

 

If you need more please provide more details of the job. Thanks.

[maestro]

Material is unheatreated A2. No draft angle, this is a vertical wall. All we have available here is cat40 VMC's, no EDM. Not really looking forward to this.

[Prototype_guy]

I personally would just go for it with what I had available...

 

I would check the part's form tolerances, like Crazy Millman says if you approach it properly and use the right toolpaths it should be ok.

 

My 2 cents worth.

[maestro]

Tolerance on this part and the mating part are a profile of .020. The gap between the 2 is .016. There is actually enough tolerance that if you used up most of it on each piece, they wouldn't even go together.

[Machineguy]

You better find out what gage sheet metal is being used. Adjust the profile tolerances accordingly.

 

Machineguy

[Machineguy]

I hope that's not the first draw for the part. Looks deep.

 

machineguy

[crazy^millman]

I personally would just go for it with what I had available...

 

I would check the part's form tolerances, like Crazy Millman says if you approach it properly and use the right toolpaths it should be ok.

 

My 2 cents worth.

 

Go for it and get the right tools and you will be fine. Give your Mastercam dealer a call and they might be able to help you out as well. X7 has doen some great things with HST toolpaths. Not sure if you company is current with Maintenance, but X8 has stepped that up even more. Learning is what most of us do in this trade. You try something and see what happens. Then you make your adjustments from there and then you have your process figured out and then on the next one have a better way to do it.

[crazy^millman]

I hope that's not the first draw for the part. Looks deep.

 

machineguy

 

I was thinking the same thing. Might be a progressive process and we are just seeing the last part of it.

 

Could also be a Hydro forming mold as well. Amazing what they are doing with that today. 24 years ago when I see it come to North Florida it was new. Seeing a 12" thick piece of rubber for the top shoe was just weird, but now many places can make some very interesting parts in one hit.

[Jayson Kramer]

There is no draft that seems strange to me on a draw die there usually some type of draft so it will pull. what is the material they will be hitting in this die?

[maestro]

I believe the material till be aluminum. Here are 2 pics of the 2 parts that work together. The cavity has a .250 ball nose end mill drawn in for reference.

[crazy^millman]

Yes I am betting in the annealed state more like a 2024-T0 maybe a 6061-T0 then it will be heat treated after it is formed. It may even been pre-soaked in a heat bath before running through the stamping operation. I have seen some different jobs over the years where this was done and surprised how well it came out. Those look like fun. Parts like that I do miss from time to time. HST those for roughing and get the finishing down and you will be surprised how well they turn out. Push the limits and you will surprised how much you learn for these parts. I cannot speak for others, but I will be glad to assist as best I can if you have a question or 2.

[maestro]

Thank you sir, I may have a question or 2 along the way.

[Micromoldmaker]

You could finish the ends with the 1/4 ball but it would be sticking out a whole bunch and chatter can be a problem on your finish. Create a boundary for the end areas each and one for the inside area. I would finish wit a 1/2 ball, maybe 3/8 ball using the middle boundary. Finish Surface Leftover the middle area with 1/4 ball with middle area boundary and use Surface Finish: Direction of Contours One Way on the end and also set Flat to 3D using the same amount of step over as your finish vertical wall.. Leave stock for a trial cut and see how your finish looks. From there you can adjust feeds and speeds to get rid of chatter and also adjust your step over amount and get the finish you want.

 

If the above is unclear see if you can put the part on the server and I'll try to generate some toolpaths so you can actually see what I'm talking about.

[crazy^millman]

You could finish the ends with the 1/4 ball but it would be sticking out a whole bunch and chatter can be a problem on your finish. Create a boundary for the end areas each and one for the inside area. I would finish wit a 1/2 ball, maybe 3/8 ball using the middle boundary. Finish Surface Leftover the middle area with 1/4 ball with middle area boundary and use Surface Finish: Direction of Contours One Way on the end and also set Flat to 3D using the same amount of step over as your finish vertical wall.. Leave stock for a trial cut and see how your finish looks. From there you can adjust feeds and speeds to get rid of chatter and also adjust your step over amount and get the finish you want.

 

If the above is unclear see if you can put the part on the server and I'll try to generate some toolpaths so you can actually see what I'm talking about.

 

Great advise.

[maestro]

Thank you. I put a file named die-cavity1.mcx-6 on the ftp site.

[Micromoldmaker]

Please remind me on how to get to the FTP site. It's been a while for me.

[Del.]

Please remind me on how to get to the FTP site. It's been a while for me.

 

 

Its under important topics that is pinned.

[Micromoldmaker]

Thanks, Del. I'll do something with it in the morning, maestro.

[Thee Rickster ™]

To ad to micro

Maybe try a Semi finish with a 1/4" .03" bull mill (waterline rest) climb mill

It won't chatter as much as ball mill

And the ball won't work as hard in the corners

When finishing

 

Leave .005 or so for finish