Sign in to follow this  
StevenL

Index Drill as a drill and boring bar (MasterCAM)

Recommended Posts

I would like to use an index drill as a drill and boring bar.  I can set it up like a drill in my tool library, but does anyone know the proper way to call it out being that its has offsets for a drill and also offsets as a boring bar.  HAAS has a video saying you can do this, but they don't really explain much beyond that.  The devil is in the details.

- The process would be call out the Drill as TOOL X with offset X and drill hole.

- Then call out "drill" again, but it's actually a boring bar now.  It would have the offset of a boring bar.  The designation would still be drill but operating as a boring bar.  This gets really confusing.  I almost think I have to do the tool as a boring bar separately using the insert on the outside like the tip of a boring bar.

Thanks,

Steve

image.png.b1aab4bf750131d24316e87eeb4ce23b.png

Share this post


Link to post
Share on other sites
3 minutes ago, StevenL said:

Then call out "drill" again, but it's actually a boring bar now.  It would have the offset of a boring bar. 

So at this point you want a different tool number ?  You will need to construct 2 tools, each with the appropriate number.

If you want the same tool number to perform one of the different "drilling" functions, select from the drop down and the Ops manager will label it with the appropriate function....i.e. drill or bore, but it will retain the same Tool #.

All drilling functions use only the H offset and so it will be the same regardless of drilling or boring. The offset is tied to the Tool # not the tool function.

This can all also be customized in the post and the new advanced drill cycle allows more complex long hand cycles.

Does that clarify?

  • Thanks 1

Share this post


Link to post
Share on other sites

For a Lathe, you only get "one tool number, per tool", but you can have more than one "offset".

T0202 > Tool #2, Offset #2 (Set only Z length, set X to 0.0 [centerline])

T0220 > Tool #2, Offset #20 (Set Z, and touch off tool in X, so that the tangent point of the insert, is the X offset.) Also, for most lathe tools, you must set a "Direction" parameter. This tells the machine "what corner of the insert you used to touch off".

Contact Haas, and ask for a copy of the Y-Axis Lathe Applications Guide. That should show you how to set up both static and live tools, in the Lathe Turret.

  • Thanks 1

Share this post


Link to post
Share on other sites

Another  solution would be to create a line drawn at the same diameter as the tool then that becomes your 1st machine profile.

So instead of the 1st op being a drill cycle it is just a turn profile. You can then use the same tool and same offsets

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites
19 hours ago, StevenL said:

The devil is in the details.

There is nothing stopping you using 2 different length offsets for the same tool in a mill, but it can be tough to "manage". On lathes its pretty obvious because all the info is in one place.

By no means impossible tho'.

  • Thanks 1

Share this post


Link to post
Share on other sites

I probably should have mentioned I was talking about a HAAS CNC lathe.   Thanks for all of the good information.  I'm going to model it again as a drill and I received  the 3D stp. file from ISCAR and I'm going to model it as a boring bar also with the proper insert.  It's going to be fun.

Thanks,

Steve

  • Like 2

Share this post


Link to post
Share on other sites
5 minutes ago, StevenL said:

I probably should have mentioned I was talking about a HAAS CNC lathe.   Thanks for all of the good information.  I'm going to model it again as a drill and I received  the 3D stp. file from ISCAR and I'm going to model it as a boring bar also with the proper insert.  It's going to be fun.

Thanks,

Steve

The Y-Axis Lathe Applications Guide that I mentioned has all the M-Codes, and NC Code samples, showing how to set up the different tools in your turret. (radial and axial tools, working on the Main Spindle or on the Sub Spindle). It is a great document for any Haas Lathe Programmer.

Share this post


Link to post
Share on other sites
37 minutes ago, StevenL said:

I probably should have mentioned I was talking about a HAAS CNC lathe.   Thanks for all of the good information.  I'm going to model it again as a drill and I received  the 3D stp. file from ISCAR and I'm going to model it as a boring bar also with the proper insert.  It's going to be fun.

Thanks,

Steve

Go on the Ingersoll site and compare your Iscar drill to theirs. Iscar bought Ingersoll for their boring heads but Ingersoll sold them at a lesser price even though they were coming out of the same building in Italy. Our Iscar guy hated it when I brought it up. :lol: The insertable drills may be the same and have the same pricing process.

Share this post


Link to post
Share on other sites
55 minutes ago, StevenL said:

I probably should have mentioned I was talking about a HAAS CNC lathe.   Thanks for all of the good information.  I'm going to model it again as a drill and I received  the 3D stp. file from ISCAR and I'm going to model it as a boring bar also with the proper insert.  It's going to be fun.

Thanks,

Steve

Nothing wrong with having 1 tool and two different offsets.

The only issue will be in Mastercam. I have found that when face drilling in lathe it does not remove the stock, so when you go in to bore with your next

op you will probably get a tool crash alarm as it does not see enough clearance for the bore bar.

This is why I suggested keeping it as 1 tool. When you profile the Drill diameter Masercam will then recognize the stock as being removed...if that makes sense.

Share this post


Link to post
Share on other sites
2 hours ago, AHarrison1 said:

I have found that when face drilling in lathe it does not remove the stock

in fact anything in C-axis, drilling or milling shows stock removal when verifying.

Your initial stock creation will have to have a hole the same dia as your drill put into it.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • 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