MSL

2020 post update issue

Recommended Posts

Hello everyone,

I’m having hard time updating some of my posts to MasterCam 2020. The issue is when I try to associate the machine/control and post to each other in the network location. I get a warning saying “This machine does not have any valid axis combinations”.

Our posts will probably work if I use default installation folder but we cannot run our MasterCam that way. I’m working with our MasterCam dealer but so far no luck with fixing this issue.  

 

10.JPG

Share this post


Link to post
Share on other sites

I've had this issue when trying to migrate posts to 2020, as well. Thankfully it was only for testing and not for all of our programmers using Mastercam, but it was a pain nonetheless. It's been awhile so I can't remember if I even fixed it or not, but it has me rethinking if we should just keep posts stored on each machine like Mastercam defaults to. I know this would make things much less of a hassle. Of course, the whole point of having them on a shared network drive is that you know that all programmers are using the exact same post. A work around here would be to use Group Policy (if your computers are on a domain) to run a logon script that could check if a post stored on the server has been updated and then overwrite local copies with the server copy. This way you would have the benefit of knowing all programmers are using up-to-date posts without breaking Mastercam's file structure.

  • Like 1

Share this post


Link to post
Share on other sites

It's been that way since 2018. There is a simple fix that was implemented for X5 and went on through 2017, GIVE EACH VERSION IT'S OWN FILE EXTENSION!

  • Thanks 1

Share this post


Link to post
Share on other sites

Somehow I need to fix this soon. I'll try contacting CNC Softwear. Is anyone with the NETHASP having the same issue?

Share this post


Link to post
Share on other sites

When you get the warning, press "ok", then go click on the "Axis Combinations" button. (next to the "Edit the Control Definition" button).

The Axis Combinations dialog will appear. Expand the "Tree" for each branch, and check X, Y, Z, and any Rotaries. (be careful, depending on how the tree is constructed, there may be a "mill table", then both rotaries, and then a "mill chuck". If you enable the "mill table", then the rotaries can be grayed out.)

You need to select all three linear axes, one or two rotaries, and then a "Tool Holding Component" and a "Work holding component". This is typically a Mill Spindle, and a Table or Chuck.

Once you enable all the components in the Axis Combination, just save the Machine Definition as normal.

  • Like 3
  • Huh? 1

Share this post


Link to post
Share on other sites

Weird...

We're running MC202 on a nethasp and we keep all our machine def's , posts and tool libraries on a network.

I've got a dozen 5 axis posts, some professionally built encypted posts and some home grown posts built from Mastercam's mpgen 5X post.

This includes a complex 5X VTL post built by Postability .

I don't mass update them with the Migration utility.

We have about 30 posts and I've been updating them one at a time as the  need arises.

I have not had any trouble with any of them

  • Thanks 1

Share this post


Link to post
Share on other sites
19 minutes ago, Colin Gilchrist said:

When you get the warning, press "ok", then go click on the "Axis Combinations" button. (next to the "Edit the Control Definition" button).

The Axis Combinations dialog will appear. Expand the "Tree" for each branch, and check X, Y, Z, and any Rotaries. (be careful, depending on how the tree is constructed, there may be a "mill table", then both rotaries, and then a "mill chuck". If you enable the "mill table", then the rotaries can be grayed out.)

You need to select all three linear axes, one or two rotaries, and then a "Tool Holding Component" and a "Work holding component". This is typically a Mill Spindle, and a Table or Chuck.

Once you enable all the components in the Axis Combination, just save the Machine Definition as normal.

Just barely got 2020 running on all of our seats today. For whatever reason, one machine definition out of 30 needed this fix. Thankfully all of that stuff is on the network......

Share this post


Link to post
Share on other sites
1 hour ago, Colin Gilchrist said:

When you get the warning, press "ok", then go click on the "Axis Combinations" button. (next to the "Edit the Control Definition" button).

The Axis Combinations dialog will appear. Expand the "Tree" for each branch, and check X, Y, Z, and any Rotaries. (be careful, depending on how the tree is constructed, there may be a "mill table", then both rotaries, and then a "mill chuck". If you enable the "mill table", then the rotaries can be grayed out.)

You need to select all three linear axes, one or two rotaries, and then a "Tool Holding Component" and a "Work holding component". This is typically a Mill Spindle, and a Table or Chuck.

Once you enable all the components in the Axis Combination, just save the Machine Definition as normal.

Thank you Colin. I will try this.

Share this post


Link to post
Share on other sites
1 hour ago, gcode said:

Weird...

We're running MC202 on a nethasp and we keep all our machine def's , posts and tool libraries on a network.

I've got a dozen 5 axis posts, some professionally built encypted posts and some home grown posts built from Mastercam's mpgen 5X post.

This includes a complex 5X VTL post built by Postability .

I don't mass update them with the Migration utility.

We have about 30 posts and I've been updating them one at a time as the  need arises.

I have not had any trouble with any of them

We have 21 different posts, only 3 of them have this issue.

Share this post


Link to post
Share on other sites
16 hours ago, Colin Gilchrist said:

The Axis Combinations dialog will appear. Expand the "Tree" for each branch, and check X, Y, Z, and any Rotaries. (be careful, depending on how the tree is constructed, there may be a "mill table", then both rotaries, and then a "mill chuck". If you enable the "mill table", then the rotaries can be grayed out.)

 

That whole "mill table" is what was causing my issue on a few machines.

We have a few machines (robodrill & matsuura's) with a 5 axis table mounted on the mill table. So when I "built" the machines in earlier versions, I put the X & Y axis, then a mill table, then the rotary axis's, then a mill chuck. Worked great till 2020. Now for whatever reason if you have the "mill table" enabled, it grays things out like Colin described.

  • Like 1

Share this post


Link to post
Share on other sites
18 hours ago, Colin Gilchrist said:

When you get the warning, press "ok", then go click on the "Axis Combinations" button. (next to the "Edit the Control Definition" button).

The Axis Combinations dialog will appear. Expand the "Tree" for each branch, and check X, Y, Z, and any Rotaries. (be careful, depending on how the tree is constructed, there may be a "mill table", then both rotaries, and then a "mill chuck". If you enable the "mill table", then the rotaries can be grayed out.)

You need to select all three linear axes, one or two rotaries, and then a "Tool Holding Component" and a "Work holding component". This is typically a Mill Spindle, and a Table or Chuck.

Once you enable all the components in the Axis Combination, just save the Machine Definition as normal.

Thank you Colin.That was the issue. All good and running now. I wish our MasterCam dealer had a knowledgeable person like you and others that always help us out here. I get lot more help here than our dealer.

Thank you all. 

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites
On 7/17/2019 at 2:01 PM, gcode said:

We have about 30 posts and I've been updating them one at a time as the  need arises.

I have not had any trouble with any of them

It's time to eat my words

I had trouble with this issue today

I updated a rock solid  home brew 5X Fanuc post and 5x drilling toolpaths were not posting correctly.

At first glance they were OK, but a closer inspection revealed dangerous output.

It turns out my machine definition for this machine was wrong and had been wrong for 10 years

Earlier versions of this post didn't care, but MC2020 did.

It took 30 seconds to fix it, once I figured it out, but without this thread I would not have had a clue where to start

Thanks Colin :thumbup:

 

  • Thanks 1
  • Like 2

Share this post


Link to post
Share on other sites
On 7/20/2019 at 5:57 PM, gcode said:

It's time to eat my words

I had trouble with this issue today

I updated a rock solid  home brew 5X Fanuc post and 5x drilling toolpaths were not posting correctly.

At first glance they were OK, but a closer inspection revealed dangerous output.

It turns out my machine definition for this machine was wrong and had been wrong for 10 years

Earlier versions of this post didn't care, but MC2020 did.

It took 30 seconds to fix it, once I figured it out, but without this thread I would not have had a clue where to start

Thanks Colin :thumbup:

 

I believe the issue has something to do with CNC Software finally "hooking up" the Generic Fanuc 4X and 5X Posts to "set" the internal Post Variables, from the MD "Rotary Component Settings".

Ever since Mastercam X was first released, the "Machine Definition" was available for Post Developers to use, however there were many features of the Machine Definition that were never "hooked up to the Post", by default. So, if you started with a Generic CNC Software Post, there were only a few items that were actually "hooked up" to read the settings inside the Machine Definition.

Most "Mill" users never had a need to use the functionality that was available in the Machine Definition, as the entire concept of an "Axis Combination" was not really applicable to the work they were doing. This is because most mill machines only have a single spindle, and a single "work holding device" (single piece of stock). It wasn't until you got into programming a dual spindle or dual turret lathe, where the concept of Axis Combinations comes into play, as a method of passing data to the Post Processor about "which tool and spindle are active".

Something is happening where "previously configured Axis Combinations" are now being reset when updating a Machine Definition from a previous Mastercam version, to 2020. It is curious for sure...

Share this post


Link to post
Share on other sites
12 minutes ago, Colin Gilchrist said:

Something is happening where "previously configured Axis Combinations" are now being reset when updating a Machine Definition from a previous Mastercam version, to 2020. It is curious for sure...

The only trouble I've had was with the drilling toolpaths

I had a 4X HBM file  that would not let me start a new drilling toolpath

I loaded the generic 4X machine def.. then reloaded my machine def and have not had that trouble since

 

MC2019 5X drilling toolpaths are NOT coming into MC2020 correctly all the time

They will come in OK, and backplot OK

Sometimes they post OK, sometimes they don't

I'll have to do further work now that I've got my old post lined out.

I'm in the process of rebuilding it, starting with a new MC2020 Fanuc 5X post

but that is not ready for prime time yet

I tried to define the machine 100% with the machine def and was not successful.

I gave up and edited the axis definitions inside the post and I'm getting correct output now 

  • Like 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