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:

Cavity surfacing suggestions/strategies?


colton_m
 Share

Recommended Posts

Hello,

 

I'm new to surfacing and would like to get some suggestions from those with more experience.

 

I have a cavity I would like to machine, about 5" wide, 3.5" deep with drafted walls and large fillets in the corners.

 

Mastercam: X7

 

Machine: 2015 Haas VF3-SS (has HSM turned on and 12,000 spindle)

 

Material: 6061 Aluminum

 

Available Tools:

- 1/2", 3/8", 1/4" ball or bull endmills.

- 1" or .75" sandvik 390 cutters.

 

I have attached a sample file with the roughing and two different finishing strategies I came up with, Could anyone have a look and make some suggestions? The finish needs to be very nice, so I'm not 100% sure that my step-down, speeds-feeds and filtering settings will give me what I need.

 

Thanks!

CAVITY SURFACING TEST.MCX-7

Link to comment
Share on other sites

Use a flat endmill for roughing, no ball.  And on aluminum you can easely go with .100 stepover

 

God I miss making molds!

 

Thanks for the comment.

 

I updated the file to use a 1/2" 3F .06" CR endmill on the roughing OP.

 

Do you think an ER25 collet would be sufficient for these speeds:

 

.006" FPT at a .100" step over would be 170ipm

1000sfm, 1/2" tool = 8000rpm

Depth of cut is at .875" right now

 

Might consider getting a 1/2" sleeve for my 3/4" hydraulic tool holder.

Link to comment
Share on other sites

Thanks for the comment.

 

I updated the file to use a 1/2" 3F .06" CR endmill on the roughing OP.

 

Do you think an ER25 collet would be sufficient for these speeds:

 

.006" FPT at a .100" step over would be 170ipm

1000sfm, 1/2" tool = 8000rpm

Depth of cut is at .875" right now

 

Might consider getting a 1/2" sleeve for my 3/4" hydraulic tool holder.

At 8000rpms I wouldn't run more than 150ipm, but if the manufacturer says your FPT is good then go for it.  Ive ran 12000rpms at 250ipm at 1.25 DOC.  The ER25 might be kinda small, try an ER32 or a solid holder.

 

Your finish tool path looks ok to me, but theres more than one way to skin  cat.

Link to comment
Share on other sites

At 8000rpms I wouldn't run more than 150ipm, but if the manufacturer says your FPT is good then go for it.  Ive ran 12000rpms at 250ipm at 1.25 DOC.  The ER25 might be kinda small, try an ER32 or a solid holder.

 

Your finish tool path looks ok to me, but theres more than one way to skin  cat.

 

170ipm @ 8000rpm and 250ipm @ 12000rpm both give the same feed per tooth at a .100" step over, so I have high hopes for that.

 

Do you know if there's a way to add shallow cuts to the Hybrid finishing toolpath? It seems to be leaving a large step over in the bottom of the cavity and on the fillets at the top of the pocket.

Link to comment
Share on other sites

 Ive never used the "hybrid" toolpath.  Play around with shallow cuts.

 

The steep / shallow tab seems to only be used for setting depth limits.

 

Under cut parameters there are 3 boxes under "step". I made some changes in there are was able to get the stepover on the floors to look a lot better.

 

It seems that the machining times are a lot quicker using hybrid because there is no overlap between steep and shallow like I had when using two finishing paths.

 

Hybrid - 118mins

Finish contour and then finish shallow - 152mins

 

Any recommendations on finishing feed rates?

Link to comment
Share on other sites

The steep / shallow tab seems to only be used for setting depth limits.

 

Under cut parameters there are 3 boxes under "step". I made some changes in there are was able to get the stepover on the floors to look a lot better.

 

It seems that the machining times are a lot quicker using hybrid because there is no overlap between steep and shallow like I had when using two finishing paths.

 

Hybrid - 118mins

Finish contour and then finish shallow - 152mins

 

Any recommendations on finishing feed rates?

By increasing the stepover to .100( stilll on the conservative side),  increasing the plunge height on entry from .015 to .03 and changing the filter settings I reduced your run time on the roughing to 42m.  

And by speeding up out feedrate on the finish to 150imp and changing the filter settings I reduced your finish runtime to 55m.

Link to comment
Share on other sites

The file opens in X9

 

I understand that but I wouldn't be able to send that file back to him or even have the same options in this toolpath. It wouldn't show me the same options so without X7 loaded I wouldn't see his file I would see the X9 version of it.

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...