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:

How To Force Alternate 5 Axis Combination?


McLaren
 Share

Recommended Posts

 Trying to figure this out and hopefully someone can help me. Mastercam 2018 is posting out

B-8.253 C0.
X10.8407 Y3.1385

But I don't have enough 'X' travel so I want to go

B8.253 C180.
X-10.8407 Y-3.1385

Any thoughts? I went into my plane manager and edited the plane by spinning the gnomon 180°, but that didn't help. Thanks in advance for any and all replies!

Link to comment
Share on other sites

Can you tell your machine def that you can only rotate so far in either direction?

I have to do that for our 5ax trunnion. By default it can go -30 to +110 deg. But I have to tell it 0 to +110 because it's pretty close to my X+ travel limit, this makes the rotation change.

Link to comment
Share on other sites
52 minutes ago, McLaren said:

 Trying to figure this out and hopefully someone can help me. Mastercam 2018 is posting out


B-8.253 C0.
X10.8407 Y3.1385

But I don't have enough 'X' travel so I want to go


B8.253 C180.
X-10.8407 Y-3.1385

Any thoughts? I went into my plane manager and edited the plane by spinning the gnomon 180°, but that didn't help. Thanks in advance for any and all replies!

Some posts have a "bias angle" is the misc variables. I don't have much success with them, but you can try. 

 

Link to comment
Share on other sites
1 hour ago, K2csq7 said:

Sometimes you can get around this with "Limits" in the multiaxis paths, if the misc values don't help. 

MT has a  checkbox on the setup branch "use alternate B axis solution" for this situation. 

I'm using Dynamic OptiRough. It's a 3+2 toolpath

1 hour ago, jeff said:

What is the B- limit value set at? Or am I way off base here.

It's at B-35 B+110. The problem is I have valid B-10.000 movements that don't need to be fixed. If nothing else I will limit 'B' in the mmd file. Just was hoping for a better path by path solution.

1 hour ago, TheePres said:

With Hass trunnion I control this with misc "primary bias". I'm not at computer so don't recall exact value I use. Try 0,1,2..see if gets you needed code

 

Looks like our post doesn't have this :(

Link to comment
Share on other sites

Also, check the Post Switch "adj2sec". That stands for "adjust to secondary", and gives the Post Processor the ability to "flip the Primary 180".

Last thing,

The "mi10$" switch can be used to "disable" negative or positive range from the Secondary, on a "per operation" basis. So you could simply set it to "2" for "Positive only", for that Operation. Since the Secondary is "limited" and "can't go negative", it should force "C180 B+".

Link to comment
Share on other sites
On 2/20/2018 at 1:49 PM, C^Millman said:

What is the toolpath? There are limits in the toolpaths, but really going to come down to what toolpaths and process you are doing to see what might be the best method to help. Where did you get your post? Can go back to the post builder and ask them to add this ability.

 Toolpath is 2D Dynamic Mill. Post is from In-House Solutions. Sounds like we definitely need to have this ability added.

On 2/20/2018 at 1:57 PM, Colin Gilchrist said:

You should be able to control this with "mi4$ and mi5$", for that particular Operation. If this is a "Null Tool Change" Op, then you must enable "bias_null" switch inside the Post.

You should just have to plug in "180" for the Primary (mi4) and "8.253" for the Secondary (mi5).

No such misc. integers.

On 2/20/2018 at 1:59 PM, Colin Gilchrist said:

Also, check the Post Switch "adj2sec". That stands for "adjust to secondary", and gives the Post Processor the ability to "flip the Primary 180".

Last thing,

The "mi10$" switch can be used to "disable" negative or positive range from the Secondary, on a "per operation" basis. So you could simply set it to "2" for "Positive only", for that Operation. Since the Secondary is "limited" and "can't go negative", it should force "C180 B+".

Again, no such misc. integer.

Link to comment
Share on other sites

What post are you using for this machine

these are standard features in the Generic Hass Trunion post that ships with Mastercam

 

# Features:
# --------------------------------------------------------------------------
# This post supports Generic 5 axis milling.
# It is designed to support the features of Mastercam X Mill
#
# Following Misc. Integers are used:
#
# mi2 - Absolute or Incremental positioning at top level
#        0 = absolute
#        1 = incremental
#
# mi3 - Select G28 or G30 reference point return.
#        0 = G28, 1 = G30
#
# mi4 - Start initial primary rotary axis bias
#       +/-999 represents start as close to limit as possible
#       0 represents calculate without using bias
#       Any other value represents an angle in degrees to attempt
#       to position near.
#        -999 = Low, 0 = Off/Default, 999 = Hi, Value = Angle bias
#
# mi5 - Start initial secondary rotary axis bias
#       +/-999 represents start as close to limit as possible
#       0 represents calculate without using bias
#       Any other value represents an angle in degrees to attempt
#       to position near.
#        -999 = Low, 0 = Off/Default, 999 = Hi, Value = Angle bias
#

 

Link to comment
Share on other sites

Yes, you need to talk with In-House Solutions, since they are the ones that built your Post Processor.

Have you read through the Post Processor Header, to read the comments at the top of your Post? Most Posts have comments at the top that describe the features of the Post, and the "controls" that are built into the Post, like the Misc. Integers and Real Numbers. These Parameters can be used by the Post to control output.

Link to comment
Share on other sites
Quote

# mi4 - Calculated 5-Axis Angles
#         0 = -A Solution
#         1 = +A Solution

this is a cut and paste from an old InHouse 5X post I have here

This is for  a JOBS C/A head head gantry mill, but I would expect to see something similar in your post

Link to comment
Share on other sites
  • 4 years later...
9 minutes ago, serge.lavor said:

Hello all here, I am new to MasterCAM and currently running 2022 version. And having exact same problem, I want my C axis be 180 flipped. But my Misc menu is different to the one you guys showed above. Please help, how do I force my C axis to be flipped? 

You should post a Ziptogo file, it is easier and also shows you are a legitimate user of Mastercam.

  • Like 1
Link to comment
Share on other sites

That looks like a Factory Thermwood Post. Reach out to those guys they can help you in no time. Ask them to give you the PDF explaining all of the different feilds so you know how to make the adjustments you need. They claim they don't have one then tell them they owe you one. I suspect mi1 or mi2, but can't be sure.

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...