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 HOLLOW SQUARE TUBE


wojtek90
 Share

Recommended Posts

On 3/29/2020 at 11:07 AM, So not a Guru said:

Create the lines that are where you want to feed.

Ccreate a point where you want the clearance to be.

Create a point toolpath by opening the Point toolpath:

Select all of these points before closing the dialog.

Move type Rapid, select the clearance point.

Select the top of the upper line.

Change move type to Feed rate, select the bottom of the upper line.

Change the move type to Rapid, select the top of the lower line.

Change the move type to Feed rate, select the bottom of the lower line.

Change the move type to Rapid, select the clearance point.

Click the OK check mark.

All done.

Directed her from another thread I started...am I able to use multiple feedrates in one point toolpath?

 

I'm trying to up the RPM and feedrate once I'm engaged in the hole.

Link to comment
Share on other sites
8 hours ago, JB7280 said:

Directed her from another thread I started...am I able to use multiple feedrates in one point toolpath?

 

I'm trying to up the RPM and feedrate once I'm engaged in the hole.

I haven't tried it, but you should be able to by using edit toolpath, after you've created it.

Link to comment
Share on other sites
  • 2 weeks later...
  • 3 years later...
On 3/26/2020 at 7:19 AM, crazy^millman said:

Here you go.

5TH AXIS DRILL 4 X 4 NO RETRACT_2019

CAD

I drew a line through the center of the holes top and bottom. I then extended the line .1 in both directions. This will act as our lead in and lead out to get the tool into the holes and out of the holes without a rapid move, but allow a rapid move between both holes to not have wasted time feeding down one line. I could have not extended the lines, but experience tells me this is needed to not crash the tool and tear something up.

CAM

I called up a basic 3 Axis Vertical Milling machine. I then called up picked Contour as my toolpath in the 2D area under the toolpath ribbon. I picked the 2 chains I drew in the center of the 1st hole which are the 2 lines. I went and grabbed a 1" inch endmill and defined it to to the machining required. I grabbed a HSKA-100 holder since I always define a holder for anything I do in Mastercam. Any programmer not defining holders in this day and age is lazy IMHO. On the Cut parameters page I turned off Comp. I changed the contour type to 3D.

I used no other settings. No Depth of Cuts, lead in/out, break through, multi passes, tabs.

In the linking parameters I unchecked clearance and retract. I set feed plane, top of stock and depth to zero. I made sure Feed Plane and Top of Stock were incremental. Depth will grey out on a 3D contour this is normal.

I then expanded the Linking parameter hitting the plus button to show Home / Ref Points. I then used 2.5 for Z absolute only for the approach and retract.

I hit the green button and now I have a toolpath doing what you asked.

This is not a drilling cycle. This is how I wrote code by hand to do this same exact thing in 1988. One of the 1st programs I wrote for a shop when I was in trade school. We didn't have NC machines or CNC machines so I wrote programs for local shops for the teacher to get experience. I wrote it was one move and it was a 12" x 12" pieces of Steel tubing with a 1" wall. The owner called the teacher screaming about the .5 ipm feed rate for 10" through the tubing. We were drilling a 4-1/2 holes with a spade bit on a big HBM. It was an easy fix, but I gave them exactly what they asked for originally. 

HTH

Thanks, I didn't pay attention to the date of the post I think it's older but, it helped

  • Like 1
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...