Locking Operations

[MadMaxx42]

Good morning

what does locking operations do

I have trouble with speeds and feeds changing

I set all my speeds and feeds in every operation....and then i code and look thru and a few have changed back to default speeds

if I click on a tool in the list in the op window.....or rename the tool all the speeds and feeds settings change sometimes and sometimes the stepovers in cut parameters in dynamic milling ops change also

i have to go thru 3 times each op sometimes to get them to stay

a whole lot of wasted time reviewing and resetting

 

i have lock feedrates set in config if i open an existiing file that setting is not necessarily checked

 

So does locking ops have any effect on keeping things set they way i have set them

 

i use alot of high performance endmills and they have to run at speeds feeds and stepovers that are the manufacturer specifies or they wont warrantee the cutter

 

Thanks 

[Leon82]

It prevents regeneration.

 

In the settings you can lock feed rates. This let's you type it into the field in the tool page.

 

Or I always put my feeds in the tool so it never changes.

[Colin Gilchrist]

As Leon mentioned, go into the File > Configuration menu > Toolpaths Page. Check the box for "Lock feedrates". (While you are there, change the Memory Buffering option to about 85%, instead of 50%)

The 'Lock Feedrates' function will make the RPM/Feedrate "locked" to the Operation, but only when the Operation has finished 'generating'.

So, if you start a new Contour Op for example, then click on different tools on your tools page, you'll see that the Speed/Feed will be updated, based on the tool that you picked. Once you have finished generating that Operation, those Speed/Feed values are now "locked" to that Operation. Changing a Tool (type or number), will not effect the RPM or Feedrates. (NOTE: you can still manually override those values, by physically typing in a new value.)

Also, if you do want to actually change to a different tool, and you want to use that "new tool's" speed and feed values, then you can Right-Click on the new tool, and choose 'Re-initialize speed & feeds'. 

[Guest]

2 hours ago, Colin Gilchrist said:

While you are there, change the Memory Buffering option to about 85%, instead of 50%)

Why 85%, I've seen others say the same thing, I always put 100%

I would put 200% if I could.

[Colin Gilchrist]

9 minutes ago, byte me said:

Why 85%, I've seen others say the same thing, I always put 100%

I would put 200% if I could.

Windows itself, the Operating System, needs some RAM to run. If you want to do other tasks while Mastercam is running. Often, this has no real bearing in the 'real-world' anymore, as I don't think the recent versions of Windows would allow a program to reserve more memory, than is truly available.

I have a feeling that this is a hold-over from the old DOS and/or Windows 95 days, more than anything. But I have (previously) had issues when pegging this to 100%.

[Metallic]

In my years of programming mastercam I have found the solution for tools is baking the feeds and speeds directly into the tool definition and manually overriding them for specific applications if necessary.

I assume others here are have a smarter way but that seems to be the most consistent for us.

I'd love to hear how others approach this topic with feeds and speeds. I do have some feed/speed chooks but that is more set and forget and the tool def level.

[Ben Wood]

 In the configuration file uncheck the box for automatically calculate HST defaults to stop the step over from changing in dynamic milling.  As others mentioned checking the box for lock feedrates will prevent the feedrates from changing.