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:

dynamic rest milling


Hertz
 Share

Recommended Posts

Hi Guys, I have lots of parts that have counterbored holes and I like using the dynamic rest mill to do the counterbore after I drill the hole. Here's the thing. I have 17 holes that need a counterbore so I drill them all one operation, but then I have to individually do each hole with a separate operation. I copy the operation but then I have to go adjust each one for the proper hole. (Make sense?)

Can I somehow select them all (every counterbore) as one operation?

Link to comment
Share on other sites

You mean with multiple passes?

Doesn't seem like the right path to do. There would be too much stop time vs the restmill path which is continuous.

Keep in mind I am not taking all the width with one cut.

 

Use the roughing option with circlemill to spiral out. works awesome. if you uncheck the helix entry the endmill will plunge into the hole then spiral out, can also add a finish path in the same toolpath.

Link to comment
Share on other sites

I like using the Helix Bore toolpaths c/bore after drilling. You can do multiple passes or single, provided your endmill is wide enough.

 

I do not want to use helical boring. Too much pressure on the tips of the endmill. Hence why I like to use the dynamic restmill.

Now as for GF8er's suggestion, I have not tried that. Would that not plunge radially every multipass? You say it spirals out? I'll have to give that a shot.

Link to comment
Share on other sites

Ok I tried the rough circle mill and it looks fine except it cuts from the middle so I end up cutting air until it reaches where the hole was drilled. Now I didn't see anywhere but does it allow me to specify the pilot hole somewhere so it doesn't cut air? Eg I'm using a 1/2" endmill. The hole is 1" and the counterbore is 1.75". When I do the circle mill rough, it cuts air until it gets to the 1" diameter.

Link to comment
Share on other sites

Why not use multiple machining regions?

 

I tried. It will only grab one as the way it works is it automatically takes the (biggest or smallest, can't remember) contour as the cut area and since they are all the same size, it only ends up doing one. Even if they were different sizes, it would still grab only one. Same with a dynamic area type toopath. You can have a bunch of islands and you can select them all and it automatically takes the first selection as cut and the rest of the selections are automatically avoidance.

Something similar to that anyway, I may not be explaining it correctly.

Link to comment
Share on other sites

Ok I tried the rough circle mill and it looks fine except it cuts from the middle so I end up cutting air until it reaches where the hole was drilled. Now I didn't see anywhere but does it allow me to specify the pilot hole somewhere so it doesn't cut air? Eg I'm using a 1/2" endmill. The hole is 1" and the counterbore is 1.75". When I do the circle mill rough, it cuts air until it gets to the 1" diameter.

 

Here's an example on how to start circle mill not from the center.

CIRCLEMILL.MCX-7

Link to comment
Share on other sites

Ok I tried the rough circle mill and it looks fine except it cuts from the middle so I end up cutting air until it reaches where the hole was drilled.

 

You could helix entry with a high angle so it gets to the bottom in no time, this will allow you to set where it starts also because of the helix radius you tell it.

Link to comment
Share on other sites

I learnt something with the circle mill example of having the ramp angle set to 0 to make the tool plunge at the specified helix radius, but we usually just do it like Jeremy with a dynamic area clearance toolpath, set your helix angle to 0 and your top of stock to the same height as your finished depth and use the helix radius to achieve the cutter start point just inside the clearance hole you have drilled. Hope this makes sense

Link to comment
Share on other sites

Ok I looked at the file Jeremy. By the way I originally DID use dynamic restmill. This is my whole point to the thread, to be able to pick multiple holes with one operation instead of separate ones. For some reason if I select them all, I get only one machined. Yours worked because you have different size holes. Make them the same and try to run the same toolpath. Gf8er I see what you did. makes sense to just adjust the radius'.

Thanks guys.

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...