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:

mmd & control files


jim1960
 Share

Recommended Posts

MC 2020.  I am trying to modify my mmd & control files and not having so much luck.  I understand the mmd is the machine and the control is the control, I wish I understood more about what each does.  My real problem right now is trying to figure out how and when I can open and modify either one is just maddening.   I guess I understand that I must have a machine group before I can have a control group.  But if I open my machine like I am going to start a tool path I can not see the group to set the default tools- speeds and feeds ect  for each tool path. If I just select the Machine Definition Icon I can modify the defaults but then get this error as I save it image.png.a1d0e5202588fcf108df71a4c9841d84.png

Any help would be appreciated, my VAR is of no help, has no clue. 

 

Thanks

Jim

Link to comment
Share on other sites

Typically when I've seen this, it's mostly been a boned update by the user from the previous version...

Sight unseen, this is just a guess but I would think updating your files again from the previous version might clear this up...BUT there's an outside chance if you did what I think you may have done, you might have corrupt versions now in the previous version as well....

Here's what I do to update to the newest version...

I create an Update folder on my desktop...

Inside of that folder, I create 2 folder structures for the previous and newest versions

2019-07-13_11-27-45.jpg.924c51a7cd8ee21f68640bb89076e922.jpg

2019-07-13_11-28-20.jpg.75f1980523368a132dc969a23528ceba.jpg

Time saving tip...I'll create the first structure and then copy and rename to the proper verison...

Then take ALL of the files you wish to update and copy them to the correct version folder...

Then use migrate and select the source folder as the previous version folder that is on your desktop and the new version folder for the destination folder...

Files that are typically copied and migrated...

.mmd

.cmd

.pst

.psb - if necessary

.tooldb

.materials

once all updated copy to the new version...as you built the folder structure, it is easy to know where it all goes back....

Some may scoff at this and say just do this or that...that's fine, there are other ways to accomplish this BUT I have been doing it this way for many, many versions.

Once the install is complete, I can be up and running in 20 minutes, few, if any issues.

DO NOT EVER migrate your config file.....copy your .workspace file for you RMB and menu layouts

 

JM2C YMMV

 

Link to comment
Share on other sites

I'm getting the same thing, Tried old bear's suggestion, not working.  Still getting same message.  I've NEVER had this issue before, ever.  I've always migrated from folder to folder without any issues and I expected this time to go just as smoothly.  nope.

 

Any more advise?

Link to comment
Share on other sites

 

This is a repost from a similar thread...

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

 

This is a repost from a similar thread...

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.

Thanks Colin!  I would never have thought of this.

 

This happens after I save.... funny I checked the axes and they were all checked, but somehow they become unchecked which is why I have to go back into machine definition again... this seems odd.

Link to comment
Share on other sites
4 minutes ago, JeremyV said:

Thanks Colin!  I would never have thought of this.

 

This happens after I save.... funny I checked the axes and they were all checked, but somehow they become unchecked which is why I have to go back into machine definition again... this seems odd.

It is odd behavior for sure.

It did not happen in 2018, or 2019, that I can recall. I believe they have been doing some work to clean up "under the hood", for the Machine Definition, and Control Definition Files, but that is just based on the behavior I've seen.

Something that is fairly interesting for those of us building Posts, is every "Machine Definition File", is basically a "Mastercam Part File", with a different file extension. This is done so you can include "geometry", especially Solids, but also Points, Lines, and Arcs.

The Machine Definition is used with Mastercam Mill-Turn, to be able to define "kinematic branches" in the Machine Tree. A "branch" is simply a collection of "machine components", with a hierarchical relationship. This means that the "Machine Base" component is always "fixed" with no movement, in relation to the "System World View". From there, each branch begins with a Component being added to the Base.

On regular Milling and Turning machines (non-Mill-Turn), there are always two branches in the tree. One is a "Stock or Work-Holding" branch. This branch must terminate with a Component that is defined as capable of holding "Stock". This is typically a "Chuck" or a "Table" component.

The second branch of the Tree is a "Tool Holding Component". This can be a Turret, or a Mill Spindle, depending on your machine type.

The beauty and power of the "Tree" comes into play when you start defining a machine with multiple Spindles and/or Turrets. This means you need the ability to tell Mastercam "which tool, spindle, and turret" is active in a particular path. For these machines, there are often 2, or 4 different "axis combinations", depending on which combination of Turret and Spindle, is active for a given Toolpath in Mastercam.

I think part of what is occurring is somehow during the update process, the check-boxes that were enabled previously are somehow being unchecked, so the automated "check for valid axis combinations" function is failing, and many users (Mill especially), have had no exposure to what an Axis Combination even does.

The place where I do use Axis Combinations in Milling, is on a 4-Axis Mill, where I want to be able to turn off the 4th Axis output, when I want to run "3-Axis Only". In that case, I will define the "default" Axis Combo as "4X", and have the 4th axis checked, along with a Mill Rotary Chuck. (Mill Table is Unchecked in this scenario). Then, I will create a 2nd Axis Combo for "3X", and have only XYZ, and the Mill Table, and Mill Spindle checked. (4th Axis and Mill Chuck are unchecked.)

 

 

 

 

Link to comment
Share on other sites
  • 2 weeks later...
16 hours ago, jim1960 said:

JeremyV

I the tree is expanded all the boxes are checked but I still get the error.

I do not know what else to try.

Jim

Which Tree???

Are you talking about the Tree inside the main Machine Definition dialog box?

We are talking about the Axis Combinations dialog, which you must press a button to launch. It has an identical copy of the Tree on the main dialog page. Hover your cursor on the row of buttons along the top of the MD dialog box, and click the Axis Combinations button.

Link to comment
Share on other sites

The migration process to 2020 rebuilds the axis combinations available for machine def. In some cases, this will turn off invalid combinations and will require you to create a valid axis combination.

Make sure that your axis Machine Coordinate dropdown is not set to Macro for axes used in your axis combos:

Macro.thumb.png.85a147732a1f78784562a7a31e9cc7dd.png

 

It is important that machine defs are cleaned up and fixed going forward, as the settings here are driving more and more things. If you're having issues with a machine def, feel free to message me and we can take a look at what's going on. 

Link to comment
Share on other sites

I guess I am still confused I can find the Axis Combinations once I am the Machine Definition Manager, but it does not look like the Machine Component Manger.  Where do I find the Machine Component Manger? 

How do I go about messaging you?

Thanks

Jim

Link to comment
Share on other sites

The possible axis combinations in Machine Definition manager are based off of what machine components you have set up, and how you have set them up, in the Machine Component manager- which you get by double clicking on any component in the machine configuration 'tree'.

1022341577_MachineDef.png.19cbffa4510b067275cb5a628c2f77ec.png

 

Jim, you can get in touch with me by clicking on my username and then clicking "Message" on the next screen, or by emailing me at [email protected]

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...