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:

Remove 4th axis A0 from Haas post


Recommended Posts

I'm sure this has been brought up a few thousand times, but I just need to remove the A0 from the g-code so I don't need to edit it. Thank you for your help. N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T215 M6
N130 G0 G90 G54 X0. Y0. A0. S305 M3
N140 G43 H215 Z2.
N150 G98 G84 Z-.525 R.1 F33.9556
N160 G80
N170 M5
N180 G91 G28 Z0.
N190 G28 X0. Y0. A0.
N200 M30

Link to comment
Share on other sites

Easiest way to do this > also requires no Post Edits.

Go into the Machine Definition Manager. Open the Haas Machine Definition. 

Press the 'Edit Axis Combinations' button. This opens the Axis Combinations dialog box.

Right-click in the white space and choose 'create new axis combination'.

Right-click > Expand all

Check: X, Y, Z, VMC Spindle, and Mill Machine Table. (Don't check the Rotary Axis.)

Name this (or rename), "3-Axis Only".

You should now have 2 Axis Combinations in the dialog. One for 4X, one for 3X.

The one at the top of the list = the default output mode. So drag-n-drop to change the order if necessary. 

Green check Mark to save the Axis Combinations. 

Save the Machine Definition. 

If needed, open the Mastercam File, and open the Machine Group Properties, then do a Replace on the Machine Definition to load the edited MD.

In the Operations > select the 3-Axis Axis Combination, and this basically "tells the Post", that you are running a 3X machine. But, if you do have a 4X job to run, then you can get 4X output. 

Technically, you could setup multiple 4X Axis Combinations, to support physically moving the Rotary and mounting it in a different orientation on the machine. (Flipping the rotary from left-to-right or right-to-left, or even aligning to the Y Axis.)

  • Like 2
Link to comment
Share on other sites
1 minute ago, poolrod2 said:

Every time I open a new Mastercam, I have to create or modify in the edit combinations, it won't save for some reason even after I move it to top top of the list.

Where are you making the change? If you are opening the Machine Group Properties > you are only making the change "locally" in your existing Mastercam File. If you want to change it permanently: go into the Machine Definition Manager, and make the Library change. Then, in any existing Mastercam File > perform a "replacement" of the Machine Definition file, through the Machine Group Properties. 

Link to comment
Share on other sites
46 minutes ago, poolrod2 said:

I don’t see a place to save it in Configuration/ Default Machines

That's not the place to make this edit. That Default Machine tells Mastercam which Machine Definition File to load "by default".

You need to edit your Machine Definition, by using the Machine Definition Manager. This is on the Machine Tab.

As long as you don't change the Name of the file you are editing, and that file is associated as the Default Machine, then the changes made through the Machine Definition Manager will be included in any new file you create. 

Something to understand > when you create a Mastercam File and load a Machine Definition (either manually, or by having a default Machine Definition assigned in System Configuration), Mastercam saves a "local copy" of the Machine Definition inside your Mastercam File. So if you edit the "Library Copy" of the Machine Definition, those changes will be "included in any new Mastercam File that you create". 

 

 

Link to comment
Share on other sites

Looks like this has been resolved, but Ive got a bit more to share on this topic for the next person.

If you are often adding and removing your 4th axis, or you're running with a 4th axis on one side of the table and a 3-axis fixture on the other side, both IKE and with MPMASTER style posts have good ways to support changing between 3 and 4 axis setups automatically.

In both cases, there is some post logic setup to detect if you are using entirely 2d and 3d toolpaths programmed in Top plane. The post will know that your only using A0 and will remove the A0 from the post. If you then post a different program that has some axis sub or cuts in the front plane, the post will detect that the A axis is needed for this job and will use A values, including A0 so you can run it on your 4th axis.

In both posts, this is the default behavior since it covers most machines, but if you always use the A-axis, even when programming everything in TOP, you can disable it.

With mpmaster, this feature is controlled in pwrtt$. In it, you will see a line that reads: 

           #sav_rot_on_x = rot_on_x    #Uncomment this line to output rotary axis value even when it's not used

uncommenting this will overwrite the lines above it, and the post will decide that A values are always needed, even if they are all A0.

in IKE, we have a switch to control this same feature:

swt_frc_rot_output       : 0           #Force rotary output even if no rotation is detected: 0 = No, 1 = Yes (Only valid for 4-axis machines)

Setting this switch to 1 will cause the post to force the A0 calls. Leaving it at 0 will filter out the A0 calls for running the machine in 3-axis mode.

  • 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...