Speeds and Feeds Settings

[render]

Hi There

Have just started using NX5 at work after previously using WorkNC. Are you able to save the Speeds and Feed values when creating a tool in the library, so you don't have to remember them everytime you create a process?

Andrew

 

[Jaydenn]

The simple answer is no; you cannot associate speeds with a tool. The speeds are associated with the operations, not the tools. Huge limitation with NX.

Search the help documentation for "Machining Data Library" or "feeds and speeds library". These are th NX solutions to automatic cutting data. That might set you on the right track.

That being said, in all my years programming in NX, I have never, ever, ever, ever been able to get satisfactory results using any of the so called "automatic" speed and feed calculators.
That's not to say they don't work... Simply that I have never succeeded in using them!

My personal method is as follows.
I create the entire NC program, from start to finish. I set up NOTHING. No speeds, no feeds, leave it all blank.

Once you are done, switch to tool view and expand all the operations within one tool. Select all the operations, right click, choose object, choose feedrates. This will globally edit the speeds and feeds for all operations within that tool.

Rinse, repeat, done.

Jay

 

[markrief]

Speeds and feeds cna be assigned directly to library tools. In the machining data libtary, go to the Tool Machining Data tab, and enter data for specific tools.

This will bypass the ususal calculations. This is useful if you always use the same cur mathods, tool materials, and part materials, or if you simply want a tool to always have the same feed and speed.


Mark Rief
Product Manager
Siemens PLM

 

[wmalan]

I would also add, you can use also use the Machining Methods as the place for this as well.

By creating a Method, I can assign feeds, speeds, stock, and intol/outol. Then just drag and drop all the operations under that Method while in Machining Methods View. It's easy to keep track feeds/speeds using Machining Methods since you can easily see the operations is using these attributes.

I find not many folks use this feature of NX especially coming from another cam system that bases feeds and speeds to a tool rather than a process. It's especially nice for us that use the same tool but with different feeds/speeds in various operations. It took me a while to come around that not always should the tool dictate the feed/speed.

--
Bill

 

[raysapp]

Bill your blowing my mind. I've never used methods for anything other than setting stock and occasionally in/out tol. I've always set speeds and feeds inside the op. The closest I've come to automating is copying ops, but that that can lead to other issues. The idea of creating a discrete array of methods specific to cut strategy, tool and perhaps even mat. would have never have occured to me.

Been thinking about creating templates for machining stainless steel, with stepovers etc. set specific to that material. To that I can now add a list of methods, like perhaps "variable pitch carbide peel mill" that allows me to program, like Jay, without having to open the speeds and feeds tab every time. Nice

It's a brave new world.

Ray S
NX 7.0.1.7

http://www.appliedprecisionproducts.com

 

[raysapp]

Oh well...spoke too soon.

You mentioned speeds but I saw only feeds. Just as disappointing feeds are not driven by feed per tooth, as I prefer. Maybe I'm missing something but I don't think "method" is quite up to the task. Too bad, it's a good idea. Like Jay I've never trusted S&F calculators. Perhaps Siemens would be open to enhancement.



Ray S
NX 7.0.1.7

http://www.appliedprecisionproducts.com

 

[markrief]

Ray,
I think what you need is available using the machining data library. It considers part material, tool material, cut method, tool diameter and lentgh. Based on these, it sets speed, feeds, depth of cut, and stepover.

The basic idea is to just enter values that you know work in your shop. The more you enter, the more accurate the results will be when you calculate in future operations.



Mark Rief
Product Manager
Siemens PLM

 

[raysapp]

Thanks Mark
I'm sure you're right.
That's a hump I need to get over... It's probably not as difficult to set up as I imagine.
My reluctance is based on the habit of having set them myself for so many years as well as an unsatisfying experience using mastercam's.
I'll give it a shot.





Ray S
NX 7.0.1.7

http://www.appliedprecisionproducts.com

 

[wmalan]

"You mentioned speeds but I saw only feeds."

Oops your right. I work in airframe multi-axis milling and we never change the spindle speed but do change feeds like crazy. We have process books that list specific feeds for each tool at certain areas on the large parts. Also, most times the same tool definition is used multiple times. For this, Methods works simple and sweet compared to the Material library. Also, many shops use multiple cam systems so they tend to create a standard non system specific process.

Given the overlap of features in NX, I'd not be unhappy to see Methods have a hook to speeds or even the Materials Manager as well.

Btw Mark, years back when methods was introduced, this is what I thought it would develop into...

--
Bill