Dynamic mill back feed rate default

[MrFish]

Anyone know why i cant change the Dynamic mill back feed rate default to anything more than 12500mm/min feed rate when setting operation defaults in X6 ?

[Mick]

Let me check Mr Fishy

 

Edit: Hmmm, yes, its the same for me here. I thought it might be some setting within the machine def, but it is limited for both the generic machine, and my current def.

 

Something internal by the looks of things..

[Guest CNC Apps Guy 1]

That's not very fast.

[MrFish]

That's not very fast.

 

 

he must be quite at work -

 

Thanks for checking Mike.

[Mick]

Mark, I'm always on the alert for any queries you may have

 

I'll make a deeper inquiry for you tonight. And no, I'm not quiet, but I always monitor what is happening

[Mick]

Double post..

[MrFish]

Mark, I'm always on the alert for any queries you may have

 

I'll make a deeper inquiry for you tonight. And no, I'm not quiet, but I always monitor what is happening

 

Thanks Mike . I have sent to QC as well, Will let you know how I get on.

[Mick]

Thanks Mike . I have sent to QC as well, Will let you know how I get on.

 

Ok, I wont bother sending to QC then

[Colin Gilchrist]

Hey guys,

 

Yes, you most certainly can change the Back Feedrate default values.

 

Here is the issue in a nutshell: The 'Operation Defaults' file that you are editing contains a Machine Definition file embedded inside the defaults file. The only way you can edit those defaults is to open the .DEFAULTS-6 file directly.

 

Try this procedure:

 

1. Open Mastercam with an empty database. (If you have Mastercam open, Save, Machine Type > Design, File > New)

 

2. Do File > Open, and set your file type to 'All Files'.

 

3. Navigate to your Ops Folder, and select the MILL_MM.DEFAULTS-6 file. Press Ok. (Shared McamX6\Mill\OPS\MILL_MM.DEFAULTS-6)

 

4. This will open the Defaults file in Mastercam, "as a MCX file". Basically it loads the file into Mastercam and give you the ability to edit your default operation parameters, along with the ability to make edits to the default machine settings.

 

5. Go to 'Machine Group Properties' and select the 'Files' tab. In the 'Machine - Toolpath copy' section, press the Edit button. This will open a copy of the Machine Definition Manager, with the default machine selected.

 

6. Go to 'Edit General Machine Parameters' and make your Feedrate limit adjustments. For example, enter 60,000 mm/min for the Max Feedrate value. Once you've entered your metric data, use the 'Convert to in./min.' button to calculate the equivalent inch values.

 

7. Close the General Machine Parameters dialog box.

 

8. Save, then close the Machine Definition Manager.

 

9. Green Check out of the Machine Group Properties dialog box.

 

You can now make edits to your Operation Default values. Since you have the file open, might as well do it here.

 

Note that this process works for specifying all sorts of default values. For example, you could go do another 'Edit' on the Default Machine, and change the min/max spindle RPM by editing the properties of the Tool Spindle component, in the Machine Configuration tree. The default Max spindle speed is '50,000' RPM, so you can change it here for the maximum in your shop.

 

Once you are finished editing the default values you want to set, you need to save the file.

 

10. Do File > Save As. Make sure you are in 'Shared McamX6\Mill\Ops', and press Save.

 

11. Do Machine Type > Design, File > New to clear out the Mastercam database.

 

12. Outside of Mastercam (in Windows Explorer), navigate to the Mill\Ops folder, and rename the MILL_MM.MCX-6 file to 'MILL_MM.DEFAULTS-6'. Overwrite the existing file.

[Mick]

Thanks for that info Colin.

 

Phew, all that just to change a default feedrate.

[MrFish]

Thanks for the indepth instructions Colin.

 

Maybe with machines getting alot faster these days this should be updated to a higher default, or better still have it linked to the machine def for the max possible feedrate, but could still be set lower in the default file - just an idea.

[Colin Gilchrist]

MrFish,

 

I'll certainly bring up the idea of adjusting some of the default values that we ship Mastercam with. The problem with 'Defaults' is that everyone wants something different. While new machine tools get faster, we have lots of customers that are still running older machines. So we change a default value from 12,500 mm/min, to 50,000 mm/min, and now we get complaints from people about defaults that are "too fast".

 

I do think we need to make it easier to configure the default settings so that all users can set the values they want. You have the ability to make the changes now, but the process is pretty involved, as you can see from the word fortress I built above...

 

Thanks for asking the question though. It's obvious that we need to put some thought into default values and how to set them...

 

Regards,

[Chris Rizzo]

Colin, can you send that perfectly detailed description in a company-wide email to every person there at cnc...just so they can see in black and white what a circus the system is.

[Newbeeee™]

Thanks Colin for the detailed explanation.

Is this in any install / help documentation? If not it should be.

Cheers

[Slixmix]

I'm using X6 MU3. I have some Dynamic Area Mill paths that I changed the back feedrates to 300. IPM from the default 100. in the toolpath parameter page but when I post it out, it's still at 100. IPM. Any thoughts?

[Alien]

I'm using X6 MU3. I have some Dynamic Area Mill paths that I changed the back feedrates to 300. IPM from the default 100. in the toolpath parameter page but when I post it out, it's still at 100. IPM. Any thoughts?

Go to Setting-Configuration-Toolpaths and uncheck Lock Feedrates.

Must help.

Sincerely,

Michael.