Bob W.

Mastercam for DMG-Mori NTX2000

Recommended Posts

On 9/16/2020 at 10:17 AM, Aaron Eberhard - CNC Software said:

I'll have to defer to someone with more knowledge as I only dabble on the MT side.  But in general, if the options are either to set a default behavior (this toolpath ALWAYS has X or ALWAYS DOES NOT have X), in the case where it's situational (I'd want X only when this AND this are true), the option is generally left off out of the box.  It's a better/more predictable experience to always have to to flip a switch because you need it on 75% of the time than to remember to turn it off 25% of the time, especially if that 25% of the time could be dangerous.

I believe that the default state of coolant commands and such are controlled by the machine environment, though, and are customizable to the users preference by the dealer, but I'm not 100% on that, so don't quote me on it :)

Do you know if there is any plan to get the misc integers, reals, and custom drill parameters into MT?  We just finished up our 5-axis bore/boss probing routine for our Makinos and it was done exclusively with post mods and custom drill cycles and parameters.  We don't even have Mastercam's probing add-in.  The probe routine will probe a feature and back calculate the offset corrections given the B and C-axis positions during probing.  We run Dynamic Fixture Offset on the mills so there are multiple offsets that get adjusted.  On the NTX we will be running TCP so it will be the same.  These features were hugely powerful and it is a big gap for MT.  I do know Esprit supports this (custom toolpath inputs) and also has custom parameters for tools which is a huge plus.  Basically tool definitions in Esprit also have ten custom parameter inputs exactly how Mastercam mill has ten misc reals in the toolpaths.  Having these inputs in tool definitions allows one that is savvy in macros to direct tool measurement/ break check routine parameters at the tool level and make them PERFECT.

On 9/14/2020 at 11:49 AM, crazy^millman said:

Everything related to the misc integers and reals is shifted in MT to the Code Expert. Once you have what you want you can set them in the consumer side to get the output you are looking for. Yes all the features can be added. Not sure about the G10.9 issue and sure hope this doesn't drag out for a long period of time.

How are these done in the Code Expert side?  Do they persist, or do they need to be reset every time a program is posted?

Share this post


Link to post
Share on other sites

image.png.663aa078a3546bfdf4882c3da741e0bf.png

This calls a macro and sends all inputs to this macro.  The macro does the rest.

image.png.effbda2d9bd999064fbbd0ca64be2623.png

  • Like 1

Share this post


Link to post
Share on other sites

Bob, I don't know the answer but I'll be surprised if we as end users ever get the kind of freedom on these posts as we did on the MP based posts

I suppose that's not to say it's not doable but it may have to kick upstairs to CNC to get that built in

Share this post


Link to post
Share on other sites

Bob,

All of the drill cycle customization is available in MT as it is elsewhere in Mastercam.  Your local reseller should be able to get the items added into your machine environment.

In the Mill-Turn platform we opted to replace the limited misc value (10 integers/10 reals shared between all toolpaths) with an unlimited number of tokens which can be used for integer, real, boolean, or string values.  The tokens can also be limited to use for specific operation types and other conditions.  I am not sure that I understand the question of whether they persist or not but I think maybe there is a misunderstanding that has occurred somewhere.  When you post from Mastercam to the sync manager you can edit any of the available tokens in the sync manager nodes, including multi-selection of operations to set similar values at the same time.  Once you have done so, click save and the data will be written back to the .mcam file.

For coolant, we opted for a strategy approach to better deal with the myriad number of coolant types that generally appear in the more complex mill-turn style machines.  The strategies allow you to finely control how the various coolant options are applied across tool changes and reposition moves.  The strategies are applied in the sync manager where you can easily visualize the work flow for the operations across the various streams.  For example, if you use the same tool in your b-axis head on your left spindle and follow with using it on your right spindle, do you want the coolant to turn off while the b-axis rotates and repositions, or do you want it to spray all over?  Do you need to enable your through spindle coolant prior to approach to allow the pressure to build before cutting and then enable your flood to turn on after approach?  Do you reverse the process for retract or do you simply turn everything off prior to retract or even after retract?  Strategies can be defined to handle any of these cases and any others that you may desire.

I will keep an eye on this thread and will try to add more information if needed. 

 

Edited by Paul Decelles from CNC Software
  • Thanks 1
  • Like 4

Share this post


Link to post
Share on other sites
24 minutes ago, Paul Decelles from CNC Software said:

When you post from Mastercam to the sync manager you can edit any of the available tokens in the sync manager nodes, including multi-selection of operations to set similar values at the same time.  Once you have done so, click save and the data will be written back to the .mcam file.

I think this answers my question whether the changes persist or not.  Once a value is assigned to a token it stays with the operation permanently once saved and doesn't need to be reset every time the program is posted.  So the work flow is such that the part is programmed as normal in Mastercam, then settings (coolant, tokens, etc...) are dialed in the Sync manager, then it is simulated, then posted.  Settings made in the sync manager will be permanent and will remain with the operations if other edits are made and posted in the future.  Sound right?

 

Share this post


Link to post
Share on other sites
1 hour ago, Bob W. said:

I think this answers my question whether the changes persist or not.  Once a value is assigned to a token it stays with the operation permanently once saved and doesn't need to be reset every time the program is posted.  So the work flow is such that the part is programmed as normal in Mastercam, then settings (coolant, tokens, etc...) are dialed in the Sync manager, then it is simulated, then posted.  Settings made in the sync manager will be permanent and will remain with the operations if other edits are made and posted in the future.  Sound right?

 

That sums it up. Have to watch though when you start really changing or adding operations since that will change the syncing process. If that has to happen the software alerts you it happened and re sync is needed in Code Meter. The cool thing is all the operations that have other assigned tokens are still in effect, but the syncing tokens have been changed. It would be no different in Mill where we have a Stock model made and then add operations before ti that effect the stock mode. The difference is Code Meter is letting you know where a stock model is none the wiser. 

Edited by crazy^millman
Grammer and Spelling Mistakes
  • Thanks 1

Share this post


Link to post
Share on other sites

Yes, token settings will persist with the operations and will be applied when posting in the future.  However, I feel that I should explain a bit further.  Machine developers are free to provide as many tokens in the sync manager as may be required for a specific machine tool.  These tokens can be set to appear in the various areas of the sync manager such as job specific tokens, stream specific tokens, or in operation specific "nodes" (start of operation, tool change, approach, motion, or retract).  The specific nodes that are available in an operation can and will vary.  For example, using a tool to cut the face of a part and then a second operation to turn the OD on the same part will result in the first operation not having a retract node and the second not having a tool change node.  This is important to keep in mind when you are adding or removing operations in Mastercam as you may need to visit the settings in the sync manager if these situations arise.

Another important point is that token settings can only be saved back to Mastercam if all operations are posted.  The idea here is that you would want to maintain your settings for the complete job while allowing token setting changes to posting single operations or selected operations without hosing your original settings.  The next time you post to the sync manager, look next to the name of the IOF file at the top of the sync manager.  A colored ball will appear there; green, yellow, or red.  Green means that the current IOF matches the data in the Mastercam file.  Yellow means you have made changes in the sync manager that have not been saved back to the part file.  Red means changes cannot be saved back - you may have either posted a single operation or perhaps made changes in Mastercam that are not reflected here.

I also wanted to clarify my earlier reply regarding custom drill cycles.  While the custom parameters are available as in the rest of Mastercam, the system has no way of knowing exactly what those settings mean so you will not automagically see a probing cycle in simulation from a custom drill cycle.

 

 

  • Thanks 1
  • Like 1

Share this post


Link to post
Share on other sites

The option to switch between radius and diameter is only tied to the upper turret by specifying G10X0 and G10x1 (be careful, it’s always diameter unless you have something special). The machine will alarm when reading G10.9 in the lower turret. I have been working with Mastercam NW for more than 2 years, and we are close to fix all issues with the NTX2000 machine environment.

Share this post


Link to post
Share on other sites
On 10/6/2020 at 11:44 AM, Mustafa-CNC said:

 

Sorry, my reply was for the G10 issue on the NTX.

 

Share this post


Link to post
Share on other sites

So we are still working on this and still having post issues, tweaks.  MCAM NW is very responsive but damn this is getting old...  The Esprit post ran the machine flawlessly IMMEDIATELY.  C'mon Mastercam, these machines have been out a long time.  Why aren't they dialed yet?  It appears the Mori AE was right, I will be dealing with this stuff for months...

Share this post


Link to post
Share on other sites

That bites Bob...I would have hoped that by now the product would be mature enough as to avoid this kind of stuff.

It's all well and great that your reseller is responsive but at the end of the day it just needs to work.

That's something that Esprit and a couple others have just been able to do....

While our Mazak was real close out of the box....that doesn't take into account that there are a plethora of other popular machines.

Good luck!!!

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