Post not recognizing back feed rate

[AndrewK]

Can anyone point me in the right direction for troubleshooting this issue? I am using a dynamic mill path and a 4-axis haas post.  Despite using the micro lift, the feed rate remains the same throughout the tool path, it does not use the feed rate I have set in the "back feed rate" input box.

Thanks!

[Colin Gilchrist]

1 hour ago, AndrewK said:

Can anyone point me in the right direction for troubleshooting this issue? I am using a dynamic mill path and a 4-axis haas post.  Despite using the micro lift, the feed rate remains the same throughout the tool path, it does not use the feed rate I have set in the "back feed rate" input box.

Thanks!

First thing I would do is "download a fresh copy of MPMaster" from this website, and do a quick test.

Open your existing Mastercam File, select "All Operations", and press the "G1" (post) button.

The dialog box will open up. Press (and hold) CTRL + SHIFT + ALT, then press the letter "P" on the keyboard. This will enable the "Select Post" button on the G1 Dialog Box, and allow you to "select MPMaster". (ignore the warning which pops up)

Does a fresh copy of MPMaster post correctly? If not > I would also check to be sure that your Cut Feedrate and your Back Feedrate, are "actually different". Seems silly, I know, but I've had it where I forgot I bumped up the actual cutting feed, and my back feed was identical, so modality made the feed/backfeed equal, and only the top-level feed was output.

[AndrewK]

14 hours ago, Colin Gilchrist said:

Does a fresh copy of MPMaster post correctly?

Yes it does! Thank you. I dug into our post a little more and found this line right near the top that seems to be the culprit.

maxfeedpm   : 50    #Limit for feed in inch/min

I changed this to 200 and it is now posting the way it should. Should this be tied to a value from Mastercam, rather than hardcoded into the post?

[crazy^millman]

1 hour ago, AndrewK said:

Yes it does! Thank you. I dug into our post a little more and found this line right near the top that seems to be the culprit.

maxfeedpm   : 50    #Limit for feed in inch/min

I changed this to 200 and it is now posting the way it should. Should this be tied to a value from Mastercam, rather than hardcoded into the post?

Depends on the age of the post and where the company you work for purchased the post from. I have seen companies carry V6 posts from 30+ years ago forward and then wonder why their post doesn't support the modern stuff in Mastercam. They get an updated post and then realize how much money they lost for all those years cheaping out and not spending money on a good post.

[Colin Gilchrist]

3 hours ago, AndrewK said:

Yes it does! Thank you. I dug into our post a little more and found this line right near the top that seems to be the culprit.

maxfeedpm   : 50    #Limit for feed in inch/min

I changed this to 200 and it is now posting the way it should. Should this be tied to a value from Mastercam, rather than hardcoded into the post?

Every Post has different features and functions. Instead of thinking "should this be done a certain way", like reading a value from the machine definition, that is totally User-Preference, and based on who built your Post.

Your Post has a bunch of features and functions. You should read through those switches, and the comments at the top of the Post, to see "how the particular Post Developer set up that Post", and what features it includes. Are you aware of the Misc. Integer and Reals Numbers? These are set at the Operation Level, and are used by the developer to control NC Code output, based on the programmer changing the input in the Operation file, and forcing a regeneration before Posting.

In general, every Post makes use of the Misc. Values, in some way. Even "in the background", based on the default values, those numbers change the code output which is written to your file as NC Code.

If you're delving into Post Editing (or configuration) > I'd highly recommend you start with MPMaster. There is a bunch of extra logic, in both MPMaster (Mill), and MPLMaster (Lathe), for things like High Speed Code output, which is just not present in the default Posts from CNC Software. But, you'll need to read through the Post, and try/test the output. Don't be afraid to setup your Ops, Post the Code, then open the Post in a text editor, change a switch, save the Post, and 'repost' the file, to see the output change.

However > MAKE A BACKUP OF THE FILE FIRST, IN A DIFFERENT FOLDER. Sorry, didn't mean to yell, but really needed to emphasize that last point. In fact, make two backups, in separate folders. Just to be sure. Also, remember that Machine Definition and Control Definition Settings, will affect Post output as well. So, back those up as well.

• Be sure to read the "How to set Control Definition Defaults" topic on the main page.
• Check my signature > I have YouTube videos called "MP 101", which covers a basic post processor class that I taught back in 2016 or 2017.

 

[AndrewK]

Thank you for the information!

[cruzila]

Speaking of copies, I always put a "safe" copy offsite just in case the building burns down. There can never be enough backup!!!

[Roger Martin from CNC Software]

An easy way to backup your Machine/Control/Post files.
With a file opened with (at least one) operation using the Machine and its related files.
File -> Zip2Go (on the backstage menu).
Make sure the proper "Machine Group types" is checked.
(Optional) You can also uncheck the "Config file" under File Options.
Now "Create file" to generate the ZIP package.
You will get more files in the output than you really need, but who cares?
You have these important ones you need backed up.

[Colin Gilchrist]

1 hour ago, Roger Martin from CNC Software said:

An easy way to backup your Machine/Control/Post files.
With a file opened with (at least one) operation using the Machine and its related files.
File -> Zip2Go (on the backstage menu).
Make sure the proper "Machine Group types" is checked.
(Optional) You can also uncheck the "Config file" under File Options.
Now "Create file" to generate the ZIP package.
You will get more files in the output than you really need, but who cares?
You have these important ones you need backed up.

Roger, a handy tip > After the Zip-to-Go File has been generated, you'll see a list of the individual files contained in the Z2G. You can manually click to select these files (using CTRL to add individual files to the selection), and then press "delete" on your keyboard. This gets rid of any of the extra files like "Operation & Default Libraries", and the Report/Config files.

I will typically strip the Z2G down to the part file, MD, CD, and PST (+ PSB, if needed).

Also, I love 7-ZIP for looking at any Zip File, because the "Flat View" option makes navigation so easy. Just drag-and-drop the files into a Windows Explorer Window, in the proper folder...