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:

Right angle head spindle direction


mwc815
 Share

Recommended Posts

We just got a used Alberti right angle head. It is going to be mounted in a Haas VF series mill. By researching the forum, I was able to set up machine def. and alter the router post to generate code that works. The one bug I can't figure out is the spindle direction. M03 spins backwards. I can call it a left handed tool to make it spin the right way, but I really hate to lie about tool definitions. Any ideas?

 

  thanks, Mike

Link to comment
Share on other sites
  • 6 months later...

Hi Guys,

 

We just purchased a right angle head.

 

if possible, could someone link or send a copy of a program as an example.

 

My plan is to drill, circle mill and thread mill or tap in the "X" axis.

 

Any help would be great.

 

Thanks

 

Just implemented a RAH on a HEAD-HEAD machine. What post are you using? Without the right post for the correct machine setup with the correct control nothing is really going to help you. I suggest you get a hold of your dealer and have them help you get it going in the right direction.

Link to comment
Share on other sites

No need to pay someone for a RAH post...

 

IF...

 

You are using a 3X machine, with a Fixed Position, RAH attachment. (Either Bolt-on, or Tool-Changed, as a tool in the magazine.)

 

The only case where you would need to have a post "build" is in the case of a "programmable" RAH. This is where you want to have "C-Axis" output, and have the program change the rotation of the head inside the NC code. (And really, the post builder just takes the 4X Router post, and converts it to a Mill Post. This is 10 minutes work tops for a decent post writer.)

 

If all you are doing is mounting a RAH, then the Machine Definition, in combination with the Generic Fanuc 3X (or 4X) Mill Post is all you need.

 

You build a 3X RAH, by going into your Machine Definition, Right-Clicking on the "Spindle" component, and "appending" an "Aggregate" component.

 

Once you've added the Aggregate Head, you need to Right-Click, and add a "station". Think of a "Station" as a specific "orientation" of the RAH. (Where does the Tool point when the RAH is mounted?)

 

With a 3X Machine Definition, with the proper Aggregate/Station/Tool defined, the only other thing you have to enable is "Translate NCI with machine aggregate" check box (inside the Control Definition).

 

That's it. No special Post required. Just start a new tool path (make sure the WCS is set to the "machine view" (or Top in a "standard" VMC configuration), and the Tool Plane is oriented to "face" the feature on your part. After starting the path (Contour for example), Right-Click in the "Tool selection" area (white space) and choose "Get angled head". As long as you've got it configured correctly inside the Machine Definition, it just "works", out-of-the-box.

 

This is one of the few "features" in the Machine Definition that does work correctly, out-of-the-box.

  • Thanks 2
  • Like 1
Link to comment
Share on other sites
  • 4 years later...

I hope this works as Easy as you say Colin. I followed Giang The Tool's video on setting up a right angle head aggregate on you tube. It worked pretty well but he says to use the mprouter post and never mentions "Translate NCI with machine aggregate". Although the code posts to the correct plane(G19 in this case) it has a lot of extra codes such many G52 offsets and extra G55 work offsets for the first tool only and then no other work offset for the other 4 tools?  I might try this all over again with what you outlined in your post from 4 years ago. Anyway back to checking the forums for more RAH info. Please reply if you know of any good resources or tips please! 

Link to comment
Share on other sites
On 7/8/2020 at 10:17 AM, [email protected] said:

I hope this works as Easy as you say Colin. I followed Giang The Tool's video on setting up a right angle head aggregate on you tube. It worked pretty well but he says to use the mprouter post and never mentions "Translate NCI with machine aggregate". Although the code posts to the correct plane(G19 in this case) it has a lot of extra codes such many G52 offsets and extra G55 work offsets for the first tool only and then no other work offset for the other 4 tools?  I might try this all over again with what you outlined in your post from 4 years ago. Anyway back to checking the forums for more RAH info. Please reply if you know of any good resources or tips please! 

Get a good post and call it a day. Did a DUM80 FD machine RAH job and got to the point I needed to spin the RAH 116.486 degrees along the Spindle Axis. None one could handle it. I  tricked it in and still got good code because the post was done correctly. I am about to put a RAH on a 90 degree head facing upside down for a customer.

Here is a screen shot of what I going to be attempting to give you an idea. The main spindle is HSK-100A.

 

Here was the DMU80 RAH Setup to give you an idea what is possible with the right post.

 

 

Edited by crazy^millman
Screen Capture removed to give more attachment space
  • Like 2
Link to comment
Share on other sites
24 minutes ago, Colin Gilchrist said:

That double RAH is hurting my brain Ron! You really earned your nickname with that one!

I love it.

Oh, and the RAH mounting in a mixed-mode Nutating Machine is no small feat either...

It's just an offset, of an offset, of an offset, right?

Funny I programmed that DMU 80 in a 3+2 process and just shifted the T-C planes the difference of the gauge length. NX guys were tripping out wondering how i was able to get that done in Mastercam.

  • Like 2
  • Haha 1
Link to comment
Share on other sites
31 minutes ago, Grievous said:

What you will do if you get a different angle head with a different length, or if your tool tip distance to spindle center will change?

You program for the tip of the tool 99% of the time in Mastercam and let the post do the work. On the DMU 80 since it was in all reality a 6 axis toolpath I had to cheat to get good code so if each tool had changed in length then I would had to make planes for that changes, but since I thought far enough ahead and made 3 tools needed all the same length then one plane worked for all 3 tools. 

I did one years ago where we had 14 different tools all ranging rom 6" to 16" in length in a RAH. They were all programmed for the 2 planes they were cutting. No different than 3+2 programming and the Tool Length was accounted for in the post and done. Each RAH presents it own challenges and like I said in this topic get a good post and don't fight more than you need to get good code. 

Link to comment
Share on other sites
43 minutes ago, Grievous said:

What you will do if you get a different angle head with a different length, or if your tool tip distance to spindle center will change?

For a Fixed Angle RAH ( tool is mounted at one "orientation" or "Station" as Mastercam calls it), you only really need two offsets. The H Offset and the D offset. The D Offset is called with G45/G46, and the H is still called with G43. You would either program on the G18 or G19 plane. This allows you to still use G41/G42 with a separate D Offset, for circular or contour motion on that plane. That way you can accommodate a range of different RAH Tools, just by using Offset Registers on the machine.

Link to comment
Share on other sites
17 hours ago, crazy^millman said:

You program for the tip of the tool 99% of the time in Mastercam and let the post do the work. On the DMU 80 since it was in all reality a 6 axis toolpath I had to cheat to get good code so if each tool had changed in length then I would had to make planes for that changes, but since I thought far enough ahead and made 3 tools needed all the same length then one plane worked for all 3 tools. 

I did one years ago where we had 14 different tools all ranging rom 6" to 16" in length in a RAH. They were all programmed for the 2 planes they were cutting. No different than 3+2 programming and the Tool Length was accounted for in the post and done. Each RAH presents it own challenges and like I said in this topic get a good post and don't fight more than you need to get good code. 

You know that if you correctly register your tool in the controller you don't need to re-post at any tool change. 

Link to comment
Share on other sites

Nice setup and that looks like a Siemens's 840D control so I will see what I can do to get customers to change their proven processes to something new that have a Siemens controls when the next project comes up that require a 5 axis head. I have never seen that on a Fanuc Control, HAAS, or OSP so not sure how it will help on those controls, but next time one of them come up I will tell the customers to look for those settings. Thank you for sharing is that HEAD-HEAD or Nutating head machine? Are the settings the same for them verses a table-table machine? 

Link to comment
Share on other sites

On Sinumerik the machine kinematic is irrelevant. Just register correctly the tool so the controller can compensate it have your succession of codes correctly and with same code will work on all of them regardless of kinematic...u can even do 5x

On a fanuc u can do it but not as easy and elegantly..

N1701
(RAD 1 WIN 1-COMPUTER COMP/DIA.5)
#601=10. 
#602=#600*COS[#601](X SHIFT) 
#603=#600*SIN[#601](Z SHIFT) 
G65P9999C180.X-#602Z#603U54.D55.(G55)
G55G90G00A0B0C0
G43.4H144D144Z8. 
X-38.5526Y12.
A0B#601
G43.1
G68X0.Y0.Z0.I0.J0.K1.R270. 
G68X0Y0Z0I1.J0.K0.R80. 
M7 
M198P6531
M9 
M301 
  • Like 2
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...