wojtek90

DRILLING HOLLOW SQUARE TUBE

Recommended Posts

It is possible to program in Mastercam through holes in square tube 4X4 x0.375   . I would like to keep drill in the same hole drilling first wall then rapid down to bottom wall and drilling bottom wall,  and then go to next hole.  

I don't like drilling top surface and then come back and lower "top stock" and drill bottom wall. I would rather stay in the hole.

I can manually modify post ,but I have 30 holes and editing each one is very painful.

Thank you.

Share this post


Link to post
Share on other sites

I would approach it with a contour toolpath and call it a day. Draw the one line on the top and the other line on the bottom for the drilling motion, but you not going to get a peck. Set the ref points to act as your Rapid Approach and Retract points. Set the toolpath correctly and it should everything you need.

Here is a link to a 2020 file with one hole done to help you along. 5th Axis Drill 4 x 4 No Retract

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

I literally just signed in to say what Ron just did...

 

3D contour...break the line,  edit the path, post and go

Share this post


Link to post
Share on other sites
7 minutes ago, JParis said:

I literally just signed in to say what Ron just did...

 

3D contour...break the line,  edit the path, post and go

Do need to edit the path the way I did it. You have a feed move through the top hole then rapid to .1 above the bottom hole and feed through then rapid all and call it a day. Rinse and repeat.

  • Thanks 1

Share this post


Link to post
Share on other sites

Thank you. I have 2019 version of Mastercam. Can you please load file in 2019 version.

Thank you.

Wojtek

Share this post


Link to post
Share on other sites

Because of my little experience with  Mastercam i do not quite understand your explanation. Can you please tell me more details.

Thank you.

 

Share this post


Link to post
Share on other sites
9 hours ago, wojtek90 said:

I can manually modify post ,but I have 30 holes and editing each one is very painful.

 

Because of my little experience with  Mastercam i do not quite understand your explanation. Can you please tell me more details.

Thank you.

 

you could  modify drilling one hole make it a subroutine and call it up at each hole location

Share this post


Link to post
Share on other sites

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 1
  • Like 2

Share this post


Link to post
Share on other sites

Thank you very much for long explanation.  I will test it today evening. Thanks again for help.

  • Like 1

Share this post


Link to post
Share on other sites

Somewhere along the way, I seem to remember doing a custom drill cycle to do this...IIRC, it was just 2 drill cycles stacked on top of one another to achieve the result.

 

Share this post


Link to post
Share on other sites
25 minutes ago, The Chipmaker said:

  You can also you that method for gun  drilling! 

I use it for Shim check and tooling checks for certain customers who still use Fail Safe and Tooling balls to check tools for extremely expensive parts. 

Share this post


Link to post
Share on other sites
On 8/27/2019 at 10:09 PM, Redfire427 said:

A ballnose endmill. It appears to be a very simple application.

 

On 9/12/2019 at 8:30 PM, Leon82 said:

I can't see the file, but if surfacing if you can use a bull endmill and get a better finish if you can fit it in your feature.

 

The center of the ball endmill isn't really spinning so you would want to tilt it if possible so get some surface footage going

 

5 hours ago, JParis said:

Somewhere along the way, I seem to remember doing a custom drill cycle to do this...IIRC, it was just 2 drill cycles stacked on top of one another to achieve the result.

 

Sorry but what is IIRC and how I can "stacked 2 drill cycles on top one another" . Can you please explain that.

Share this post


Link to post
Share on other sites

Thank you very much I was able to open file and see exactly what you mean.  I do not see however in backplot rapid movement. Maybe this will be in the post.

Share this post


Link to post
Share on other sites
15 minutes ago, wojtek90 said:

Thank you very much I was able to open file and see exactly what you mean.  I do not see however in backplot rapid movement. Maybe this will be in the post.

Do you have "Rapid Moves" actually "visible" in the Backplot options dialog box? It is a "toggle" which can be turned on/off. 

Share this post


Link to post
Share on other sites
36 minutes ago, wojtek90 said:

Thank you very much I was able to open file and see exactly what you mean.  I do not see however in backplot rapid movement. Maybe this will be in the post.

You are correct it didn't rapid in 2019 or 2020. You will have to do as John recommend and use the toolpath editor to get a rapid move in between the holes. Might be best looking into the other suggestions mentioned. Sorry I thought it was rapiding in between the holes and it is not.

Share this post


Link to post
Share on other sites

A point path is perfect for this. Just add a point, above the hole, where you want your clearance height. Then create your point path.

(TEST)
(COMPENSATION TYPE - COMPUTER)
N1 T17 M06 (1/2" JOBBER DRILL)
(MAX - Z1.05)
(MIN - Z-2.17)
S764 M3
G0 G17 G90 G54 X9. Y0.
G43 H17 Z1.05
M8
Z.05
G94 G1 Z-.3575 F6.11
G0 Z-1.7625
G1 Z-2.17
G0 Z1.05
M9
M5
G53 Z0.
G53 Y0.
G90
M30

TUBE_DRILLING.mcam

  • Like 1

Share this post


Link to post
Share on other sites

Thank you very much. That is what I need.

The only problem is how can I do it for all holes by programming it entirely in Mastercam and get the post for my Haas machine rather then copy and paste each hole using your test code.

Share this post


Link to post
Share on other sites
22 minutes ago, wojtek90 said:

Thank you very much. That is what I need.

The only problem is how can I do it for all holes by programming it entirely in Mastercam and get the post for my Haas machine rather then copy and paste each hole using your test code.

Did you look at the Mastercam file?

 

Share this post


Link to post
Share on other sites
11 hours ago, So not a Guru said:

Did you look at the Mastercam file?

 

Yes I did. 

But there is the the only "Point cycle" and there is only point location and nothing about depth parameters and other parameters. Consequently when I posting it is not giving me all parameters which you give me as example. So if you kindly can show me how you did entire post I would  appreciated.

Thank again

Tube screen.jpg

Share this post


Link to post
Share on other sites

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.

  • Thanks 1

Share this post


Link to post
Share on other sites

MC2021 public beta 3at the 5:40 mark

 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

Thank you very much. That all I need. Very informative and easy to follow. You guys make my day.

Share this post


Link to post
Share on other sites
17 minutes ago, gcode said:

MC2021 public beta 3at the 5:40 mark

 

Can I get this public version of Mastercam 2021 to test my holes please? I have licensed version of Mastercam 2019  and 2020 no load to computer yet.

Share this post


Link to post
Share on other sites
46 minutes ago, wojtek90 said:

Can I get this public version of Mastercam 2021 to test my holes please? I have licensed version of Mastercam 2019  and 2020 no load to computer yet.

Yes 

you will need to go to www.Mastercam.com and create an account

To do that you will need to be on a computer that has your hasp plugged in or is connected to your nethasp

you will not need current maintenance to create an account

you will need current maintenance to download and install Public Beta 3 which you can find

here

  • Thanks 1

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

  • 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