Colin Gilchrist

ProTip: How to set Control Definition Defaults

Recommended Posts

Just found this....days after installing 2018 and spending the better part of 2 hours setting up what needed to be done.  Better late than never i guess, thanks Colin!

 

I have 10 CD's for the machines I program. 3 of the CD's use different operation defaults due to them being horizontal. Hopefully it doesn't revert anything for those 3 on the next upgrade...

Share this post


Link to post
Share on other sites
On 9/28/2015 at 10:52 AM, Colin Gilchrist said:

Setting the "Default settings for control type"

Colin, when setting the defaults for control type, can I do this for each of my different machines (VF6 3x, VF10 3x, TM2 3x, VF4 4x, UMC750 5x, etc), or does setting the defaults on one "mill type" machine override the defaults for all of my "mill type" machines?

Share this post


Link to post
Share on other sites
47 minutes ago, So not a Guru said:

Colin, when setting the defaults for control type, can I do this for each of my different machines (VF6 3x, VF10 3x, TM2 3x, VF4 4x, UMC750 5x, etc), or does setting the defaults on one "mill type" machine override the defaults for all of my "mill type" machines?

You only get one set of "Defaults" per "control type". This is why I always recommend a 1-1-1 relationship between MD-CD-PST files. Trying to have one Control Definition "do it all" just isn't practical in the real world.

Share this post


Link to post
Share on other sites

I have 1-1-1 with all of my machines, but they are all "mill" types not router or lathe etc.

So, as long as my MD, CD & post files are all named the same and assigned to one another, then I can save the defaults per your template. And that will preserve each machines control defaults, correct?

I'm about to install 2018, so I'm hoping to keep it as painless as possible. :)

Share this post


Link to post
Share on other sites

Yes.

Go into each CD, with your 'linked Post Processor' selected in the drop down menu. (Should show a green check mark). Check all of the pages, make sure all the setting are 100% how you like them.

Save those settings.

Then, select the drop down menu, and choose "default settings" in the drop down.

Go to the 'Tools' page, right-click, import > all pages.

In the dialog that pops up, choose your existing CD file.

That will bring up the dialog to import the data. Choose your existing Post from the list. This will tell Mastercam to import all the settings from your "linked post" into the Default Settings.

Now, save the Control Definition Defaults.

When you run the Migration to 2018, every single Control Definition setting will match what you setup in 2017, and will match 100% of the time, every time you update to a new version.

  • Like 1

Share this post


Link to post
Share on other sites

Thanks for this information Colin!  Years ago I made "print screen" snap shots of all pages of all my CD's and each new version of MC I installed, had to compare and change.  We have 30+ machines and had to do this for every one as they all have their own little differences.  As you can imagine, this took some time. 

You will save me oodles of time for every next new release!!  Thanks again! 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites
On 10/16/2017 at 6:55 PM, Camelot said:

Thanks for this information Colin!  Years ago I made "print screen" snap shots of all pages of all my CD's and each new version of MC I installed, had to compare and change.  We have 30+ machines and had to do this for every one as they all have their own little differences.  As you can imagine, this took some time. 

You will save me oodles of time for every next new release!!  Thanks again! 

Your situation is exactly why I made this post in the first place. So, every new release means 30 Control Definition files to review. Each CD has something like 15 pages. So 450 pages worth of settings to review, every time you update...

Setting the CD Defaults will eliminate any issues with updating, now, and into the future. I love using the 'Transition' function, because it just seemlessly updates all the files, and the next version is basically plug and play. Not having to chase down post problems does kind of take the fun out of it though...

Just kidding. Not having settings change on you when updating is ideal of course.

  • Like 1

Share this post


Link to post
Share on other sites
On ‎10‎/‎21‎/‎2017 at 11:44 PM, Colin Gilchrist said:

Your situation is exactly why I made this post in the first place. So, every new release means 30 Control Definition files to review. Each CD has something like 15 pages. So 450 pages worth of settings to review, every time you update...

Setting the CD Defaults will eliminate any issues with updating, now, and into the future. I love using the 'Transition' function, because it just seemlessly updates all the files, and the next version is basically plug and play. Not having to chase down post problems does kind of take the fun out of it though...

Just kidding. Not having settings change on you when updating is ideal of course.

Hi Colin.  Now you hooked me into asking you what the "Transition" function does.  It sounds like some kind of magical button.  Maybe you have talked about it in an earlier post.  If so, let me know and I will search.  I don't want you taking more time than you need teaching us idiots.  lol. 

  • Like 1

Share this post


Link to post
Share on other sites

Hi Camelot,

Sorry it has taken me a while to get back to you. I saw your question when you originally asked it, and I intended to reply, but got side-tracked.

The Migration Wizard is used to "update" all of your Mastercam Files, from the previous version you were using, to the version you are updating to. It can be used to update all kinds of different "library" files, but the most important of those for a regular user are the Machine Definition, Control Definition, and Post Processor files. A close second would be Tool Libraries, Operation Defaults, and Operation Libraries.

The process of using the Migration Wizard is pretty straight forward, but I must warn you: YOU SHOULD MAKE SURE ALL OF YOUR "DEFAULT SETTINGS" ARE SET IN THE CONTROL DEFINITION FILES, BEFORE YOU START THE UTILITY!!!

Otherwise, using the Migration Wizard won't really gain you anything. You'll still have to go through the CD settings for each MD/CD/PST combo, and make the necessary changes. Setting the CD Defaults, means you don't have to do that anymore, and the update will be seamless.

Migration Wizard

The Migration Wizard is simply a series of dialog box pages, that walks you through the process of updating your files from a previous version, to the current release. Typically, there are options to "migrate" from up to 3 versions back. So in Mastercam 2018, the last version you can Migrate from would be Mastercam X8. If for some reason you had to migrate from an earlier version, then you would need to install an older version of Mastercam, run the Migration Wizard in that older version, and then do it again in 2018.

For example, to go from X5 to 2018:

  1. Install Mastercam X8, and Mastercam 2018.
  2. Run the Migration Wizard in X8, to update all the files from X5 to X8.
  3. Then, run the Migration Wizard in 2018.

Ok, so how do I use the Migration Wizard?

File (Backstage View) > Convert > Migration Wizard.

There are two different "methods" to use. There is a "Basic" method and an "Advanced" method. With the Advanced Method, you get more options to filter the "types of files" that get updated.

Running Migration Wizard

  1. First, make sure you are starting with an "empty" Mastercam Database. To do this, go to the MACHINE ribbon, and choose "Design" to put Mcam into "design" mode, then press "File > New". (Using "design" mode means Mastercam loads with "no machine definition" selected.)
  2. File > Convert > Migration Wizard.
  3. Pick "Advanced".
  4. In the "File Locations", you are given the option to Migrate "Shared" Mastercam Files (MD/CD/PST/Libraries), and "My Mcamx Files" (Mastercam Part Files). You can choose one or both of these options. For me, I typically only select "Migrate shared mcamx files", because I don't want to update all my "Part" files. I will only update "Part" files on an individual basis. Running the Migration Wizard on your part file can take a loooooong time.
  5. Click on the "Migrate shared mcamx files" checkbox. The wizard will give you a "default" Source Folder, and "destination" folder. Typically, this will be "Shared Mcam2017" > "Shared Mcam2018". You can choose different Source and Destination Folders. This can be useful, if for example, you are running your Shared Files on a Network Configuration.
  6. After you press "Next", you are presented with a list of "File Types" to be updated. You can deselect the main "file types" checkbox, which removes "all" the check marks. Then you can go through the list, and pick only the files you want to update. At a minimum, I recommend selecting "Control definitions", "Machine definitions", and "Posts files". You can choose to update "all" of them, but it does take longer to run the wizard if you do this, so be forewarned.
  7. Finally, after you pick the "types" and press "Next", you are given the choice of "which version" to update from. (Again, it only goes 3 versions back...)
  8. When all your choices are made, press "Next", review the "info" page, showing your selections, and press "Finish".
  9. Mastercam will now go through the automated process of updating all of your files.

If you have previously set all your CD Default Settings, the Migration process will be smooth as silk. All your CD's will be updated with the new "static" file paths, pointing to "shared Mcam2018", and the CD will "import" all of the settings "automagically" from the CD Defaults. If you didn't set the CD Defaults, then you have to go through each page, of each CD, and make the changes manually, which is terrible.

Share this post


Link to post
Share on other sites

After talking with another forum member (Nick), there was some confusion about one aspect of "Setting the CD Defaults".

You will notice, if you open your Control Definition (through the CD Manager), that you can only edit the "Post Text Strings", when you have actually "linked" your Post to the CD.

In other words: you cannot set the "Default Post Text Strings", when you are editing the "CD Defaults" in the Control Definition Manager!

This makes it a little confusing, when you go to setup a new Post.

So, in general, you should add a couple more "steps" to the process of editing the CD Defaults.

  1. Start by following the advice in the previous posts in this thread, about "setting the Default Values", before linking your Post, or "copying" the "Linked Post Values" into the defaults. (Either method will get you to the same results.)
  2. After you have "set the Defaults", you can "Link" your Post Processor. When you do this, the "CD Settings" apply to that "specific Post", in "that specific File Location". It is important to understand that these paths are Static File Paths, not Dynamic Paths!
  3. With your "Linked Post" selected (in the Posts Drop-Down), make sure your PST file is CLOSED.
  4. Now, in the CD Manager, go to the Post Text Section, and edit all of your String Names, and Values. This will "write" that data to the bottom of your PST File.
  5. Once you've got everything "set" the way you want it, Save and Close the CD Manager.
  6. Now, Open your PST file in the Mastercam Code Expert Editor, and scroll to the "Post Text Section", at the bottom of the PST file.
  7. Manually Copy the "Post Text Strings" from your "Linked Post", and Paste them into the "Default Post Text section. (highlight the "linked text", Press CTRL + C, highlight the "Default Post Text", and press CTRL + V to "overwrite" the old stuff with the copied text strings.)

That should be it. Now, those default Post Text Strings are saved "with the Post", since there is no way to "set them" in the CD Defaults. (A big oversight in the design of the CD Manager, from the very beginning of the Mastercam X Series of software...)

Share this post


Link to post
Share on other sites

Colin,

You did an excellent job on describing in detail how to go about this.  Very easy for me to follow.  Thanks for your teachings sensei!!

 Very much appreciated!!  I can't wait to try it out on 2019 version.

Cam

  • Like 2

Share this post


Link to post
Share on other sites

JEEZE... ALL I WANTED TO DO IS CHANGE DEFAULT X HOME POSITION FROM 10 TO 8.  I THINK I WILL JUST CHANGE IT FOR EAVERY SINGLE TOOL EVERY SINGLE TIME  MANUALLY.

 

Share this post


Link to post
Share on other sites
On 8/24/2020 at 5:14 AM, MJPESTALITZ said:

JEEZE... ALL I WANTED TO DO IS CHANGE DEFAULT X HOME POSITION FROM 10 TO 8.  I THINK I WILL JUST CHANGE IT FOR EAVERY SINGLE TOOL EVERY SINGLE TIME  MANUALLY.

 

Edit that in the machine definition and should be good. 

Share this post


Link to post
Share on other sites
On 8/24/2020 at 8:14 AM, MJPESTALITZ said:

JEEZE... ALL I WANTED TO DO IS CHANGE DEFAULT X HOME POSITION FROM 10 TO 8.  I THINK I WILL JUST CHANGE IT FOR EAVERY SINGLE TOOL EVERY SINGLE TIME  MANUALLY.

 

You're in the wrong thread if you're looking to change the Home Position. That is done through the Machine Definition. This thread is about the Control Definition Defaults. Crazy Millman correctly pointed out that Home Position is set in the Machine Definition. So you could absolutely edit that file, and any new Mastercam file you create would then use that X8. Output. 

If you already have a Mastercam file with multiple Operations, you can use Edit Common Parameters to change all the Home Position values at once.

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