Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Machining a slot in inconel


Recommended Posts

You didn't mention if it was blind or a window?

It is possible, but depending on the tolerance and surface finish it might be more hassle than just making an electrode and burning it. Burning it will take longer, but at least you can just set it and forget it on the sinker instead of fiddle farting around worrying about hotdog endmills in Inconel.

  • Thanks 1
  • Like 1
Link to comment
Share on other sites
41 minutes ago, Sticky said:

You didn't mention if it was blind or a window?

It is possible, but depending on the tolerance and surface finish it might be more hassle than just making an electrode and burning it. Burning it will take longer, but at least you can just set it and forget it on the sinker instead of fiddle farting around worrying about hotdog endmills in Inconel.

It is blind. width and depth are +/- .005. Finish is 125 or less.

Link to comment
Share on other sites

Have fun with that one....  I'd say sink that thing.  Definitely less aggravation.  I've never ran endmills that small in 718.  I've been doing some seal grooves lately with .078" tools, but they are shallow and those tools are stumpy.  That gives enough grief.  I can't imagine trying to do what you are looking to do, without burning through a tool or two.  If you do end up machining them, I'd really like to know the process and tooling you settled on.  That's good spankbank material right there.

Link to comment
Share on other sites

I mean, that's only 13:1, Depth to Diameter, on the finished feature. Piece of cake, right?

That would be a difficult slot, in Aluminum.

In Inconel 718? oof...

I'm with Peter, I would drill out as much of that material as possible, without letting the holes intersect. 

Then I'd look at getting a .047 diameter endmill, from Harvey Tool, and have them relieve the neck. I would get at least 3 different lengths of tools to finish the slot. If you try to go with a single "length" to rough and finish, you'll be there for days.

I'd go with a 5X (.250 to shoulder), and a 10x (.480 to shoulder), and get an additional 10x cutter, that is ground back to .658 to the shoulder. ( 14:1, D2D, on a .047 endmill)

I'd look to finish with at least a couple different lengths of tool. For the bottom of the slot, I'd try a 1 mm diameter, with 1 mm length of cut, and 17:1 D2D. You could try something like a 1.25 mm diameter (.051), and try to interpolate a slot that is .0004-.0008 wide, to stay under your .055 width tolerance, but what a pain.

You'd be far better served by drilling out as much material as possible, and just sending it off to get burnt out on the EDM.

As slow as EDM is, you will get the part finished much faster than trying to dial in a slotting process with multiple tools that are extended way beyond the practical limit.

 

  • Like 4
Link to comment
Share on other sites
On 9/17/2019 at 11:07 AM, Colin Gilchrist said:

You'd be far better served by drilling out as much material as possible, and just sending it off to get burnt out on the EDM.

curious a little on your idea here. I'd guess the EDM speed wouldn't be terribly effected if it burnt from solid or had it pre drilled.

I'm assuming you know more than me.

Link to comment
Share on other sites

Edm will definitely go faster with less material to remove. But it is faster and easier to make two electrodes, and you likely would want to make two electrodes anyways, so removing material via drilling ahead of time would be of little practical benefit. Besides, drilling inconel sucks.

  • Like 1
Link to comment
Share on other sites
Just now, Sticky said:

Edm will definitely go faster with less material to remove. But it is faster and easier to make two electrodes, and you likely would want to make two electrodes anyways, so removing material via drilling ahead of time would be of little practical benefit. Besides, drilling inconel sucks.

This is basically what I was going to say before Sticky beat me to it. Rough/Finish electrodes, and be done with it. And yes, drilling Inconel, especially 718, is terrible.

  • Like 1
Link to comment
Share on other sites

My guys literally scrapped a set of inserts for a mold today because they were trying to pre mill some areas out before burning. I told them not too, our new fangled sinker with a rougher and finisher electrode would blow through those features faster than milling them - they didn't believe me...

They do now, but I'm the one that has to pay for it😖

The new high speed Z style flushing on the higher EDM's is pretty slick for rib features.

  • Sad 1
Link to comment
Share on other sites
On 9/18/2019 at 7:02 PM, Colin Gilchrist said:

And yes, drilling Inconel, especially 718, is terrible.

In comparison to other materials, yes.  But it can be done with a relatively high level of process security.  It just depends on what you are trying to do.  Generally speaking, drilling in 718 is fine up to 8xd or 2" deep, whichever you hit first.  Depths less than that are easy peasy as long as you don't get greedy.  You just need the right tool for the job.  We have three drilling platforms that are very capable of removing 718 material, good, better, and best.  I won't advertise here, but if you would like to know which I speak of, please feel free to ask.

Now, tool cost to drill 718, well that is a completely different story, it can get pricey, fast.  But then again, isn't mechanical material removal by all methods expensive in nickel based super alloys?

Link to comment
Share on other sites
2 hours ago, huskermcdoogle said:

In comparison to other materials, yes.  But it can be done with a relatively high level of process security.  It just depends on what you are trying to do.  Generally speaking, drilling in 718 is fine up to 8xd or 2" deep, whichever you hit first.  Depths less than that are easy peasy as long as you don't get greedy.  You just need the right tool for the job.  We have three drilling platforms that are very capable of removing 718 material, good, better, and best.  I won't advertise here, but if you would like to know which I speak of, please feel free to ask.

Now, tool cost to drill 718, well that is a completely different story, it can get pricey, fast.  But then again, isn't mechanical material removal by all methods expensive in nickel based super alloys?

Hi Husker,

Please shoot me over any info you'd be willing to share in a PM.

I typically go with Titex Drills for Inconel. Actually, for any high-nickel material, they are usually my go-to. I've also had good luck with both Mikron Tool, and Guhring, but none of those manufacturers are "cheap" solutions.

I usually find that Cobalt Drills last longer in 718 than carbide, but perhaps my cutting parameters aren't ideal on the carbide. Through-Spindle Coolant also really helps, but can be hard to feed through small drills, depending on size of the coolant holes, the type of holder (sealing), and the PSI of the pump.

Link to comment
Share on other sites
On 9/18/2019 at 4:08 PM, Sticky said:

My guys literally scrapped a set of inserts for a mold today because they were trying to pre mill some areas out before burning. I told them not too, our new fangled sinker with a rougher and finisher electrode would blow through those features faster than milling them - they didn't believe me...

They do now, but I'm the one that has to pay for it😖

The new high speed Z style flushing on the higher EDM's is pretty slick for rib features.

We need an emoji for "I feel your pain"... I didn't feel right about "liking" your post, so I clicked the "sad" button instead.

Link to comment
Share on other sites
On 9/23/2019 at 7:23 AM, huskermcdoogle said:

In comparison to other materials, yes.  But it can be done with a relatively high level of process security.  It just depends on what you are trying to do.  Generally speaking, drilling in 718 is fine up to 8xd or 2" deep, whichever you hit first.  Depths less than that are easy peasy as long as you don't get greedy.  You just need the right tool for the job.  We have three drilling platforms that are very capable of removing 718 material, good, better, and best.  I won't advertise here, but if you would like to know which I speak of, please feel free to ask.

Now, tool cost to drill 718, well that is a completely different story, it can get pricey, fast.  But then again, isn't mechanical material removal by all methods expensive in nickel based super alloys?

 

i'm also interested in your 3 drilling platforms..

Link to comment
Share on other sites

Generally speaking here is what I lead with.  I'll just post it up here as people are interested.  I'll let you guys figure out who I work for now if I didn't already spill the beans before.  Should be pretty obvious.

From around .5" to .625" and less I will lead with solids either our GOdrill or Y-Tech drills.  Above that size mark, depending on depth requirements I'll switch to KSEM.  This is in Inconel anyway.   Non S materials, I would be using KenTip FS above about .250".

The GOdrill is the low cost solution of the two solids I like, the Y-Tech can be and usually is looked at as a problem solver.  Now, I have found the GOdrills to work in just about any material, key is looking at the chips and making adjustments to the parameters to optimize.  I just ran an 8xd 8mm full depth without pecking at 85 SFM, and .0018" feed.  Could it be faster, sure likely, but our chips looked good and the drill doesn't look used after 8 holes.  It has a little trouble getting the chips out for the last .5" or so, but it doesn't seem to show up in the hole finish.  This drill has a marginless design so it doesn't rub, but this also means that if you damage the point, it may have a tendency to walk a little bit.  If this becomes an issue, that is when you enter in with the Y-Tech drill which is a 3 margin design, this cuts down on drag vs a 4 margin design, but yet still provides extra guidance and stability.  The Y-tech has a slightly different point geometry, but it is more optimized for S type materials.  This drill also is better at evacuating chips at the longer depth to diameter ratios.

For the bigger holes, I suggest the KSEM platform.  Plain and simple, it just works.  As long as you have a good stable part, you can go well over an inch and diameter with this tool, there are flat bottom geometries as well (FEG).  FEG's aren't ideal for Inco, but work very well in Titanium, Steels, and Cast Iron.  For normal angled drill points, I suggest the SPL point, it makes a beautiful hole in Inconel.  The SPL point should now have a margin-less first margin and a normal secondary margin for stability.  This reduces drag and work hardening of the wall if you have to counter-bore the hole or something after, not to mention the reduction of heat generation, which we all know likes to destroy any and all cutters.

Anyway, got to run.  If any of you would like to run any of these drills, or have tried and failed in the past.  Feel free to reach out to me and we will see what we can do to help.

Husker

  • Like 1
Link to comment
Share on other sites

I've had pretty good luck with Nachi SG-ESS PM drills in inconel, but I mostly work with inconel sheet these days. I have a 4.15mm drill that I get about 500-600 holes out of before I have to change it. Only feed it at 1.5 IPM, but it runs all day. Can even get away with pecking if you have your parameters set right.

I guess if you're doing billet work, your setup is solid, and you're using appropriate entry/exit feed rates carbide is ok, but have to make sure you're dropping feed on breakthrough or you're going to lose the lip of your drill real quick. Any sort of vibration and your drill is toast too. Tried many different carbide drills in sheet metal parts, keep coming back to the powdered metal.

Though regarding husker's post, once you get up to sizes where you can use through coolant, replaceable tip drills work alright. Have a narrower range for speeds and feeds, but not hard to dial them in. Slightly less susceptible to chipping out on breakthrough due to the HSS body having a little give to it. I think we have a couple parts with larger holes I have a ken-tip set up for.

Link to comment
Share on other sites
On 9/25/2019 at 5:25 AM, huskermcdoogle said:

This reduces drag and work hardening of the wall if you have to counter-bore the hole or something after, not to mention the reduction of heat generation, which we all know likes to destroy any and all cutters.

Haha. Yeah I know it's kinda counter intuitive, but better relief and sharper positive rake seems to work better for inconel due to it's tendency to work harden.

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...