When Copy/paste operations the speeds/feeds remain

[Doug Overkill]

I am using X6 and when I copy and paste an operation which I usually do for spot, drill & tap operations to ensure they are linked to the same geometries. First I create an operation and select all the holes and setup my spot drill. Then I copy & paste that op. When I go into parameters and change the tool for the new op to be the drill, the speeds and feeds remain from the spot drill. The same thing happens if I change tools. If I program a contour with a 1/2 mill and then notice a corner radius requires a smaller tool, switching the tool and the speeds and feeds don't update from the newly selected tool.

 

I am sure I am just missing a switch somewhere but can not find it. Any help?

[Guest]

Right click on the tool, reinitialize speeds and feeds

[crazy^millman]

There is also the lock feed rates. Setting under toolpaths that might also influence what is going on. If it is checked which I think it is by default uncheck it and see if that makes a difference. I do not use this option since I make libraries of tools with my set speeds and feeds and want that to control my speeds and feeds and not something I did one time in one operation that might have been special

[Doug Overkill]

Jparis - That seems to work, but you have to do that each time to each tool? How do I make Reinitialize the default when switching tools?

 

CarazyMill - I also have a tool library with all my preferred speeds and feeds. I want to select a tool and have those values used everytime for that tool. This is what happens when I create an operation and select a tool. What is happening is when I change a tool after an operation is created the speeds/feeds from the original tool remain after different tool is selected from library. Most common is after copying spot drill operation. I would change to peck cycle and select drill from library. What I want is the speed/feed from drill data in library to become active as it had in previous versions. What is happening now is the spot drill speed/feed remain until, as JParis pointed out, you reinitialize the tool.

[Guest]

You uncheck the Lock Speeds and Feeds as point out

 

Then when you select a new tool it will read the new tools values that you have saved to the library

[Doug Overkill]

where is the "Lock Speeds and Feeds" check box?

[crazy^millman]

Top of the screen are the drop downs. Settings then in that drop down is Configuration or you can hit Alt+F8 at the same time. That will pop up the Mastercam Configuration Dialog. Navigate down to the toolpaths in the tree on the right. On that place you will see all the different check boxes. Right above the drop down Setup Sheet Program is the Lock Feed rates check box. If checked uncheck and you will want to hit the Blue plus button to apply this. Then close. Now see fi the behavior is still doing what you were seeing or now acting like what you would expect.

 

Believe it or not people like this option and I am like you see no need for it, but what the option is there for those that do. You can put it back like you were use to or you can make it like this that some people think helps them.

[Doug Overkill]

That is exactly what I was looking for. THANKS

[crazy^millman]

Couple minute call to your dealer problem solved. 2 hour process through the forum problem solved. Glad we were able to point you in the right direction.

[Hertz]

Thanks for that as well. I know exactly what Doug is talking about. I always thought it was just a bug of some sort. Never really asked about it. Glad I read this topic.

[Thad]

I am using X6 and when I copy and paste an operation which I usually do for spot, drill & tap operations to ensure they are linked to the same geometries. First I create an operation and select all the holes and setup my spot drill. Then I copy & paste that op. When I go into parameters and change the tool for the new op to be the drill, the speeds and feeds remain from the spot drill. The same thing happens if I change tools. If I program a contour with a 1/2 mill and then notice a corner radius requires a smaller tool, switching the tool and the speeds and feeds don't update from the newly selected tool.

 

I am sure I am just missing a switch somewhere but can not find it. Any help?

 

You really need to look into making an operations library for these kind of things. I have all ream, tap, c'bore, pocket, contour, contour-ramp, etc operations saved for each different tool. Taps/reams are saved for the standard depths...just selected geo then drag geometry from op to op. Pockets/contours all have the appropriate step down, step over, lead in/out, etc. Each operation has it's comments already set, only requiring minor editing.

 

I've even gone in to settings that I don't normally use and put some good values that I would use *if* I decided to enable it. For example, in my contour-ramp op, If I'm already using this op for a 3/8 end mill, then I need a plain old contour op with the same end mill, I'll copy the op and change the contour type to 2D and enable depth cuts. My depth cut value is already there for me. It's a huge time saver!

 

Yeah, you can setup some of this in the defaults file, but you have WAY more control using an ops library.

 

Thad

[Hertz]

That has nothing to do with it Thad. I too have libraries set up for each material and each type of cut like yourself. When copying a toolpath eg spot drill then change the copied tool for a normal drill, the speed and feed of the normal drill(whiuch is set in my library) does not update when lock feedrates is selected. In other words it ignores the speeds and feeds you have set in your library.

The OP mentioned that already in his 2nd post.

[Gary]

God I need to take the time and do that. Nice.

You really need to look into making an operations library for these kind of things. I have all ream, tap, c'bore, pocket, contour, contour-ramp, etc operations saved for each different tool. Taps/reams are saved for the standard depths...just selected geo then drag geometry from op to op. Pockets/contours all have the appropriate step down, step over, lead in/out, etc. Each operation has it's comments already set, only requiring minor editing.

 

I've even gone in to settings that I don't normally use and put some good values that I would use *if* I decided to enable it. For example, in my contour-ramp op, If I'm already using this op for a 3/8 end mill, then I need a plain old contour op with the same end mill, I'll copy the op and change the contour type to 2D and enable depth cuts. My depth cut value is already there for me. It's a huge time saver!

 

Yeah, you can setup some of this in the defaults file, but you have WAY more control using an ops library.

 

Thad

[Thad]

That has nothing to do with it Thad. I too have libraries set up for each material and each type of cut like yourself. When copying a toolpath eg spot drill then change the copied tool for a normal drill, the speed and feed of the normal drill(whiuch is set in my library) does not update when lock feedrates is selected. In other words it ignores the speeds and feeds you have set in your library.

The OP mentioned that already in his 2nd post.

 

It has EVERYTHING to do with it. Having an ops library like mine eliminates the need to copy a spot toolpath and change it to a regular drill, therefore the problem never rears it's ugly head.

 

EDIT: Note that I'm talking about operations libraries and you're talking about tool libraries. That's where you're missing the point.

 

Thad

[within a thou]

That has nothing to do with it Thad. I too have libraries set up for each material and each type of cut like yourself. When copying a toolpath eg spot drill then change the copied tool for a normal drill, the speed and feed of the normal drill(whiuch is set in my library) does not update when lock feedrates is selected. In other words it ignores the speeds and feeds you have set in your library.

The OP mentioned that already in his 2nd post.

 

I think what Thad is trying to explain is if you create Operation libraries for a 1/2-13 tap you would have spot, tap drill , chamfer than tap. So use import to import all 4 of those "operation files" and drop and drag your geo into those not copy and paste a operation than grab a second, third forth tool.

 

I do what Thad does workls like a charm especially if you can get your engineering department to standardize tap depths, cbore depths and stock for facing operations and so on.

[Thad]

Exactly.

[MrFish]

Couple minute call to your dealer problem solved. 2 hour process through the forum problem solved. Glad we were able to point you in the right direction.

 

This depends on your reseller !!

[Hertz]

I see what you mean. Sorry for the confusion.

[jeff]

This will help me out a lot also!

I would use Thad's way, but when I copy/paste toolpaths, they are so random that it wouldn't really apply to my situation.

But it's definitely a handy way to make quick work of stuff!