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:

Screw on Endmills *Long reach*

dstryr
 Share

Recommended Posts

dstryr Newbie

dstryr

Posted
Posted

Picked up a new customer and they are throwing some challenging parts at me. 4"-6" deep pockets with 1/4 corner radius with a 1/4 radius fillet at the bottom of the pocket. The webs between the pockets are .060 thick. Right now I'm roughing with long solid carbide tools but I saw a post by a member of a different forum a while back in the archives about his luck with the screw on type endmills. His application was 1" dia about 18" long

Is anyone using these for deep pocketing? Will I do better than long shank tools? Right now I'm rotating between Destiny tool and Helical Solutions cutters.

Link to comment
Share on other sites
crazy^millman Veteran

crazy^millman

Posted
Posted

Maybe some with some defib technology in them will so what you are after. Ph Horn comes to mind, just not sure of the reach of their solid carbide tools. 6" deep with 1/2 endmills in Aluminum I have no problem tackling. Now come back with a .06R in a 6" deep and I will ask what engineer needed his hands slapped with the ruler. J/K

  • Like 1
Link to comment
Share on other sites
dstryr Newbie

dstryr

Posted
  • Author
Posted

Maybe some with some defib technology in them will so what you are after. Ph Horn comes to mind, just not sure of the reach of their solid carbide tools. 6" deep with 1/2 endmills in Aluminum I have no problem tackling. Now come back with a .06R in a 6" deep and I will ask what engineer needed his hands slapped with the ruler. J/K

 

What is your strategy for these parts?

Right now this is my process

 

Drill a 1" hole in the center with an indexable drill.

Go in with a 3/4 and rough it all out within .030

Go in with a 1/2 with 2.250 reach and get what I can to .010 stock

Finish 1/2 with 2.250 reach comes in and finishes

Go in with a 1/2 with 4.0 reach and get what I can

Finish with 1/2 with 4" reach

 

I was thinking something like a sanvik but not sure if they go down that small?  Or if its worth straying from carbide.

Link to comment
Share on other sites
Newbeeee™ Community Regular

Newbeeee™

Posted
Posted

I never like to use 1/2" tools in 1/4" Rad Corners. I MUCH prefer a 12mm tool. I can at least interpolate an arc in there.

 

JM2CFWIW

you Yankee boys will go metric yet!

 

For the 1/4 radius, 1/4 bottom: If you can tweak the geo to allow a bit of tool movement - say make the corner rad 0.255" this would help.

I would tend to flat the top, drill the corners on the correct arc points down to 1/4 from the bottom, and then drill out the rest with a reduced shank 1/2" ball nose. If you use a G73 with .01" pecks, and stay off the bottom by a couple of thou.

Then when you finish profile, it will whisker the bottom.

 

What I would also say (and not being a smart arse) - is that this type of work can be soul destroying. It can eat time and tooling, and you can quickly loose your shirt on it

So your initial statement of 'picked up another customer and they're throwing me challenging work' I would question - has their other suppliers dropped the work because of difficulty or can't make money on it or are you too cheap!

Just be careful imo.

Link to comment
Share on other sites
dstryr Newbie

dstryr

Posted
  • Author
Posted

 

What I would also say (and not being a smart arse) - is that this type of work can be soul destroying. It can eat time and tooling, and you can quickly loose your shirt on it

So your initial statement of 'picked up another customer and they're throwing me challenging work' I would question - has their other suppliers dropped the work because of difficulty or can't make money on it or are you too cheap!

Just be careful imo.

Ive done quiet a bit of work like this but normally it was maybe a project every couple months. This new customer is like a new project every couple weeks with very similar parts. I was hoping to invest in some tooling to make it easier but seems like investing in some 12mm cutters would be the way to go.

 

There is plenty of money there....Just wanted to invest in my process :)

 

I thought maybe the screw on cutters offered some sort of devibe that would be worth it.

Link to comment
Share on other sites
The Cathedral Newbie

The Cathedral

Posted
Posted

We use Iscar Multi-Master endmills when we have to do pockets like that. Milling a 1/2" slot 4" deep in 316ss, I use a .472" feedmill-style tip to rough and a .472" bull-nose to finish the walls and fillets. Works like a champ, especially since EDM is out of the question. These would be my first stop when looking into tools for your type of work.

 

Just make sure you look into getting a quality tool holder as well.

  • Like 2
Link to comment
Share on other sites
xycnc Newbie

xycnc

Posted
Posted

I have had good luck with them. +1000 to carbide shank. also use a metric shank and a Inch thread on head to give me added or extended relief. I feel its a good thing to have in your toolbox. Might not always be the fastest but at times it will get you out of a jam.

Link to comment
Share on other sites
P B Newbie

P B

Posted
Posted

Good quality shrink holders are the only way to go. We use them all the time  very seldom use collet chucks (got lots of them collecting dust)

Shrinks are a bit of an initial investment, but last for ever when looked after and extend cutter life

 

Did I hear right ????? America and metric in the same sentence :)

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
Go to topic listing

  • 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.

Useful Links

Contact Info

Subscribe to eMastercam News

 

Legal

Privacy Policy

Store Terms & Conditions

Forum Guidelines

Follow us

×
×
  • Create New...