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:

Drilling out pocket


Henry
 Share

Recommended Posts

No need to draw points !

Use toolpath->surface->rough->plunge .

Works with surfaces and solids or NCI file .

 

PS if you don`t have surfaces or solid , it`s not hard to bulid them.

 

Nci file is a nice feature.

A quote from help file

quote:

The plunge path is the pattern the tool takes in the rough plunge toolpath. You can select one of the two following options on the Rough plunge parameters tab of the Surface Rough Plunge dialog box.

 

¨ NCI creates a plunge toolpath from a NCI file. For example, create a pocketing routine to clear a cavity, then select the pocketing operation as the NCI to provide a pattern for the plunge path. The graphic below shows an example of a plunge path retrieved from an NCI file.

 

 

 

¨ Zigzag creates a plunge pattern in a back and forth motion. The graphic below shows a zigzag plunge path.

 

 

 

Note: When using NCI as the plunge path, set posting to Off for the source operation (

Main Menu, Toolpaths, Operations, right-click, Posting, Off).

Related Topic

Plunge rough toolpaths


PS I drilled cavities with an end mill from NCI file .

Iskander teh drill dem all !

 

[ 07-24-2003, 06:26 AM: Message edited by: plasttav ]

Link to comment
Share on other sites

We have tried plunge milling about 2 years ago. The machine was a horizontal Mitsubishi (M-H50E).

It looked great on the computer screen. One problem that we ran into was vibration. We needed to cut out thru pockets in Royalloy stainless. Plates were big: 15x20x2.375 and pockets were 9.625x14.500. It was too unpredictable for lights out production... I'm sure it would work much better on a vertical, or having the center of gravity lower. Has anyone out there used this method for a while?

Link to comment
Share on other sites

Drilling is the fastest way to remove stock in most cases....

 

robk.....I think its all in the tool design.

Iscar has some highfeed tools that are designed to keep pressure on the tool to dampen chatter....

 

If I had to cut a pocket like the one you discribed, I would just support the

slug so it wouldnt fall out and hit the table.

 

Then I would just take a 1" flat inserted mill and just do a ramping cut only around the parimeter of the pocket leaving about .1 for the final pass. The final pass would be a little scary but if you used a piece of wood or some sort of a pri-bar to keep the slug from squeezing in on your cutter when you were on the final leg of your cut, you would be fine smile.gif

 

I guess you could always drill a hole in the middle of where the slug would be and bolt it down biggrin.gif

 

Murlin

Link to comment
Share on other sites

I've dropped many a slug and it works great. The only time I use a pry bar is on extremely heavy slugs. And that is scary if the wrong person is doing it, I have seen people pry the wrong way??? An option I started using was coming back with a slightly smaller cutter to cut the last .050" and then there are no worries. Try to have the start point near the middle of the peice, error to the side of having more mass ahead of the cutter instead of behind.

 

 

HTH

Link to comment
Share on other sites

Murlin,

 

Iscar is the cutter we tried. The tool was great, but it did not suit the application (that was according to the rep. after running the tool). Originally we used to slug the pockets (additional locators in the center of the slug with screws holding it to the tombstone).It was time consuming, and the chips still had a hard time evacuating even with air blow... Right now we use 2.5" Iscar Feed Mill,and machine out the pocket clean. The time is an awesome 24 mins. per plate, and the inserts last through four plates without any problems... Again our main issue was lights out production that was safe (any such thing ?) and efficient, and plunge milling was not it. cheers.gif

 

Rob

Link to comment
Share on other sites

Robk....Thats pretty good time on cutting those pockets, specially in SS smile.gif

 

As far as lights out....the only way I go home for the night is when I am running a finish cut with a small mill that will break if anything happens.

 

I dont know if I would ever walk away too far from high feed roughing...you never know when you are going to bite a chip and break your tool.

 

You are right about the chips on cutting out a slug. Have to use alot of air to keep em out.

 

Hrmmm so those Iscar plunge mills didnt work eh??

Figures....everything always works on paper though biggrin.gif

 

Murlin

Link to comment
Share on other sites

+1 on the plunge milling. We bought a 2" Iscar "plunge" mill, and it worked great. The material was cast iron, the machine a Haas. Unfortunatly the part was more rigid that the Haas, but I found that for roughing, z-axis moves can take a hell of a bigger bite that x-y's. biggrin.gif If you'd like, I could dig up the model number of that Iscar cutter....

Link to comment
Share on other sites

Murlin,

 

No, no... The Iscar plunge mill would have worked great on a vertical, or a horizontal that was more rigid ( bigger pallet, or a smallet part that was closer to the bottom of the tombstone). This machine has a 500mm pallet, and the cener of gravity is way up there eek.gif . We have tried cutters from a few manufacturers, and for the past few months have been roughing out the pockets at night using the Feed Mill from Iscar. Knock on wood, but no crashes happened. biggrin.gif

 

Rob

Link to comment
Share on other sites

Henry,

 

Is your geometry comprised of 2D wireframe or surfaces? Is it a 2D pocket or does it have an odd shape to the floor and walls? Have you tried a simple drill grid pattern with the limits of your pocket being half the drill dia.? The Surface-Rough -Plunge works great if you have surfaces. There is even a way to rough out the pocket with Plunge using Helixes instead of a drill point pattern. In both cases, Mastercam will have a parameter for distance between centers of points. To overlap the drill, supply the distance value as something less than the diameter of the drill. HTH cheers.gif

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...