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:

Integrex Shaping option


Spotterhphc
 Share

Recommended Posts

Hey, 

I did a search and couldn't find anything on this topic. I am looking to use the shaping option Mazak offers on my Integrex i300. The feature on the part is just a simple o-ring groove that is 1.37" major diameter ( correct terminology for grooves? ). Not very big at all.

My question is, has anyone ever written a program for Shaping before and willing to share some sample code? I've been studying the manual trying to make sense of it buuuuttt...... 

The groove will be machined at B90.° so  the C axis will not be used except to position the groove top surface. It's just a flat O-Ring Groove.  

I'm working on getting the Shaping Option as we speak. The Orbiturn option I do not believe is necessary. 

Thoughts/concerns?

 

Thanks for the help!

Link to comment
Share on other sites
10 minutes ago, Spotterhphc said:

The groove will be machined at B90.° so  the C axis will not be used except to position the groove top surface. It's just a flat O-Ring Groove.  

If this description is accurate...you can mill it with contour and appropriate lead in/lead out setting all day...no shaping necessary.

You're stating the C axis moving is not necessary...position B & C to the correct location and  mill away.

It's an Integrex, it's a Mill 1st, a lathe 2nd

 

Link to comment
Share on other sites

So my plan is to use a Face Groove Tool, Sandvik#  CXS-06F150-6215AR. I can't use this tool without Syncing the Mill spindle Speed with what would be my YZ at B90. Currently I am using an Endmill to generate this feature but I have to go back through and sand the O-ring to give it a circular finish per print. So a face groover would give me this finish. My reason for thinking shaping is because the actual Spindle speed would be like 10rpm or something all the while keeping the tool outer tip at the correct diameter.

Thanks for the timely responses! 😀 

This is essentially what it's needs to do. This is the Orbit option but its similar.

 

Or are you  saying just figure out my SFM that I want and my center point of arc and then find my Feed based on that? If that makes sense. 

Link to comment
Share on other sites
53 minutes ago, JParis said:

I'd just mill it and call it day...

That's just me I guess

We don't have that option when a circular finish is called out. That is not a circular finish on the seal joint will fail under high pressure and things start exploding real quick after that. Might think about a Contour Facing head with set limits. You can engage them with a positive stop block and then it will spin out to the stop block and then retract.

https://cogsdill.com/products/zx-systems/facing-contouring-heads/

https://itstooling.com/its_products/contour-facing-head/

Some of our customers use these to accomplish that task.

http://www.wohlhaupter.com/products/facing_and_boring_heads/

 

  • Like 1
Link to comment
Share on other sites

Well I tinkered with it for a little bit and was able to hand program it. Pretty Simple when it cam down to it. Just make sure you don't have any spindle and feed overrides active and don't feed hold.  Not sure if .MOV attachments work but here is a quick clip. 

 

N3401 T34 T0 M6 (0.236 FLAT ENDMILL)
(F71.484)
(OPERATION NO - 1)
G10.9 X0
M901
M200
G91 G00 G28 X0.
G17 G90
G54 
M108 M212
B90. C90.
M107
M19S180.
G68.2 P1 X0. Y1.9827 Z0. I0. J90. K90.
G53.1
G97 
G43 H#3020 X.5689 Y0. Z.25
G17
Z.2
G94 G01 Z0. F25. M51
G02 X.5689 Y0. Z-.005 I-.5689 J0. F71.484 S20 M3
X.5689 Y0. Z-.01 I-.5689 J0.
X.5689 Y0. Z-.015 I-.5689 J0.
X.5689 Y0. Z-.02 I-.5689 J0.
X.5689 Y0. Z-.025 I-.5689 J0.
X.5689 Y0. Z-.03 I-.5689 J0.
X.5689 Y0. I-.5689 J0.
X.5689 Y0. Z.005 I-.5689 J0.
G1 Z.17 F50.
G00 Z.25 M9
M5G69
G91 G28 X0. Y0.
G28 Z0.


 
  • Like 4
Link to comment
Share on other sites
2 minutes ago, Spotterhphc said:

Well I tinkered with it for a little bit and was able to hand program it. Pretty Simple when it cam down to it. Just make sure you don't have any spindle and feed overrides active and don't feed hold.  Not sure if .MOV attachments work but here is a quick clip. 

 

N3401 T34 T0 M6 (0.236 FLAT ENDMILL)
(F71.484)
(OPERATION NO - 1)
G10.9 X0
M901
M200
G91 G00 G28 X0.
G17 G90
G54 
M108 M212
B90. C90.
M107
M19S180.
G68.2 P1 X0. Y1.9827 Z0. I0. J90. K90.
G53.1
G97 
G43 H#3020 X.5689 Y0. Z.25
G17
Z.2
G94 G01 Z0. F25. M51
G02 X.5689 Y0. Z-.005 I-.5689 J0. F71.484 S20 M3
X.5689 Y0. Z-.01 I-.5689 J0.
X.5689 Y0. Z-.015 I-.5689 J0.
X.5689 Y0. Z-.02 I-.5689 J0.
X.5689 Y0. Z-.025 I-.5689 J0.
X.5689 Y0. Z-.03 I-.5689 J0.
X.5689 Y0. I-.5689 J0.
X.5689 Y0. Z.005 I-.5689 J0.
G1 Z.17 F50.
G00 Z.25 M9
M5G69
G91 G28 X0. Y0.
G28 Z0.

 

IMG_2772.MOV
 

Yup pencilcam #1. 

Your approach vector is scary haha.

Link to comment
Share on other sites

Excellent work sir. :thumbsup:

You could program that with a contour toolpath and use switch in the post to get the output. Reach out to your dealer and provide them the sample you worked out and they should be able to get you sorted out pretty quick.

Might think about 3 or 4 passes at the final depth to get a nice finish.

 

Link to comment
Share on other sites
2 minutes ago, byte me said:

Yeah, you have to be brave.

Going slow and watching everything you have a good idea. Worse thing could happen is break a tool. That happens you figure out what you did wrong and try again. You break another tool then try something different. Try, Try and Try again and learn ways not to do something. Then you learn so many other things that help you to hone your craft. to get it right.

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...