metric machine definition

[MSL]

Hi,

We have a Makino IQ300 milling machine that is set to run in metric. The person who has been running this machine is going to retire by end of this month. He uses a different CAM software to program this machine.

I want to use MasterCam and started editing a post for it but I’m not sure how to make a metric machine definition for this post. I contacted our reseller but they said they can not make a metric machine definition. I'm sure we did it when I took Colin's class.

Can someone help me with creating a metric machine definition for my post?

Thank you.

[Colin Gilchrist]

4 hours ago, MSL said:

Hi,

We have a Makino IQ300 milling machine that is set to run in metric. The person who has been running this machine is going to retire by end of this month. He uses a different CAM software to program this machine.

 

I want to use MasterCam and started editing a post for it but I’m not sure how to make a metric machine definition for this post. I contacted our reseller but they said they can not make a metric machine definition. I'm sure we did it when I took Colin's class.

Can someone help me with creating a metric machine definition for my post?

Thank you.

 

 

The Reseller couldn't help? That should be reported to the CNC Software Post Department, so that particular Reseller can be trained.

Technically, a Machine Definition is just a Mastercam File, with a different file extension. But there is a fairly easy way to convert a Machine Definition File between unit systems, if you have a file that you want to convert.

Start in Inch Mode.

Use the Machine Definition Manager to open your MD.

Check the Metric values in General Machine Properties. Perform a Save As, and save the MD File. (Change the MD name to include 'MM' in the new File Name.)

Press the green check mark to close the MDM dialog. (This leaves the MD file open in the Mastercam database.)

Open the File Menu > Configuration. Change the configuration file from the Inch Default, to the Metric configuration file. 

Press the green check mark to complete the change to the Metric config.

It will ask if you want to scale geometry. Say Yes!

Now, go press File Save.

It will ask with two radio buttons, if you only want to save geometry, or if you want to write the file to a Machine Database. Choose the 2nd option (machine database.)

Really, unless you are running Mill Turn, or a Post with Machine Simulation output, it doesn't much matter if you use a Metric or Inch MD. Because no real 'geometry' is saved in the MD File.

The other option is to build a new MD, by starting with a Metric configuration file loaded, open the MDM Dialog, and open the Metric Machine Components file (GMD?), and build a new Kinematic chain. One branch must end in a Spindle (tool holding component), and the other must end with a Mill Machine Table. 

Your table group should be machine Y, machine X, then Mill Machine Table.

Your spindle group should be machine Z, then Mill Spindle.

The only stuff that is read from the MD, by default, is:

• The 4th Axis settings (if a Rotary Component is attached)
• The Axis Combination(s), top is default
• Coolant settings (type, plus strings[maybe])
• Operation Feed Rate limits (set at OP level)
• Min/Max Spindle Speed limits (set at OP level)

Anything else in the MD, must be added by the Post Developer, to use additional MD data.

[MSL]

Hi Colin,

Thank you very much for your detailed explanation. I get more help here than our reseller.

[Colin Gilchrist]

2 hours ago, MSL said:

Hi Colin,

Thank you very much for your detailed explanation. I get more help here than our reseller.

I'm glad it helps!

In my description above, when I mention "Check the Metric values"; what I mean is to examine all of the Metric Parameter Values, and be sure they are set to match your preferences, for driving the machine in Metric.

For example: you can configure Mastercam to use the "Home Position" in the Toolpath Dialogs, to use a location relative to the active WCS Origin, to act as a "Tool Change Location". Same is true in Lathe, and here is an important point:

In the Axis Combination dialog box, after you have created your different Axis Combinations, each separate Axis Combination has separate settings for both "Home Position" and "Reference Points". That means you can set different XYZ (mill) or DZ (lathe) Home Positions. You can also do things like create 4 different "4-Axis Mill Axis Combinations", and assign each one a different Home Position, which you could then use to mimic the Tool Change location, relative to the Active Work Offset. When you do this, keep in mind that you are describing 'relative locations' to the WCS Origin in Mastercam. Mastercam doesn't know anything about your machine, but it is a powerful tool that lets you do a lot of things to visualize your machining process, even without the use of Machine Simulation. Heck, I want my Backplot to show me absolutely as much information as I can possibly get. Using Home Position  can give you that flexibility. However, the issue comes up that when using Tool Planes, I think the Home Position Values are relative to the active Tool Plane coordinates, which means those values are rotated, compared to the real machine positions. So be careful when trying to use this in anything other than 3-Axis mode. But on a Lathe machine, for example, you can configure the Home Position for each Axis Combination (think 'Separate Turret' here), to retract to a safe Tool Change Location. If you define your Tailstock or Steady-Rest boundaries, and the Home Positions, you get some "collision awareness", where Mastercam will go "up and around" a defined boundary. This can be really nice to avoid crashing your machine!

By the way, I've put some of my old class videos up on YouTube. I'll be uploading most of the videos I have recorded over the years to that platform, as it allows you to host the video content "for free", where advertising is the mechanism that supports so much video content.

[MSL]

10 minutes ago, Colin Gilchrist said:

I'm glad it helps! By the way, I've put some of my old class videos up on YouTube. I'll be uploading most of the videos I have recorded over the years to that platform, as it allows you to host the video content "for free", where advertising is the mechanism that supports so much video content.

I went to Eapprentice website first but the website is not working!!!  I did visit your YouTube channel too. Thank you for doing it. I'm kinda rusty on editing post. I'm sure I will have more questions regarding this post. I will output them here.

Thank you.

Ara.