Z level constraints

[jeffl]

I was wondering if MC was able to control feedrates at different Z levels within an operation such as surface finish contour.

[Guest CNC Apps Guy 1]

Sure there is. You have to understand how to use the toolpath editor though.

[jeffl]

how do i get to the toolpath editor? I can edit my nc file, but I would like to select point in MC9 file.

[Guest CNC Apps Guy 1]

Open up the operations Manager, right click on the NCI operation you'd like to modify. You have several optiond on how you'd like to apply the changes, by point, by pass, etc....

 

Stolen from MC Help...

 

quote:

---

The Toolpath Editor gives you a fine level of control over the motion in a toolpath. You can make modifications to the tool motion created by Mastercam and change the way areas of the toolpath are machined. For example, the Toolpath Editor can be used to add points, then assign tool-up and rapid moves to those points, which modifies the toolpath to avoid crashing into a clamp.

Changes made with the Toolpath Editor are not associative. After using the Toolpath Editor, Mastercam automatically locks the NCI file for the operation to prevent overwriting the changes with toolpath regeneration. For more information on locking the NCI file, see the related topics below.

 

Open the Toolpath Editor by right-clicking on the NCI icon for a toolpath or by choosing Options

, Toolpath Editor from the right-click menu in the Operations Manager.

Notes:

 

¨ Be sure to make all other changes to the toolpath (such as tool or parameter changes) before using the Toolpath Editor. Toolpath Editor locks the toolpath and prevents regeneration.

 

¨ The Toolpath Editor is not available for drill or manual entry toolpaths.

 

Choose a topic below for more information.

Setting up the toolpath editor (toolpath editor options)

Toolpath editor tips

Moving a point in a toolpath

Adding a point to a toolpath

Editing toolpath point parameters (Mill)

Editing toolpath point parameters (Lathe)

Removing a point from a toolpath

 

Removing a section of a toolpath

Removing a pass from a toolpath

Removing a cut from a toolpath

Locking and unlocking an NCI file

---

Help is quite helpful and I can't really say it any better.

 

HTH

[Jimmy Wakeford from Barefoot CNC]

You may also try out the highfeed button in the ops manager. It calculates feeds by material being removed.

[EX-wccprogrammer]

¨ Be sure to make all other changes to the toolpath (such as tool or parameter changes) before using the Toolpath Editor. Toolpath Editor locks the toolpath and prevents regeneration.

 

 

This is why I do not use this feature.

[Guest CNC Apps Guy 1]

WCC, that's why you need to dial the settings first, THEN edit the toolpath.

 

Just part of the process.

[EX-wccprogrammer]

Back in the day, there used to be a c-hook called Colorfeed... No more?

[Guest CNC Apps Guy 1]

I believe that Dave Freidman(sp???) wrote that C-Hook. I've not seen it in a long while. Circa V5 or so. I'll ask him if he still has it. It may not work anymore due to the massive changes to the Database since them.

[Fig sign]

What I would do: copy your operation needed ammount of times ,and change depth of milling absolute to limit milling to the steps by Z .Change in every operation feeds and speeds to your taste .

Make regen

HTH

[Steve Biehl - Cimquest Inc]

i think the highfeed option is the easiest way to get different feedrates on the plunges. you could probably play with the settings enough to get just changes on plunges and not other moves.

[Steve Biehl - Cimquest Inc]

actually thought of another way.

 

in the feed output section of your post, do this:

 

...

if motst = 4, #Z only motion

[

feed = feed / 2

]

...

 

you would want to use a user variable for the feed output, but the point is to test for Z only motion with the motst variable.

[EX-wccprogrammer]

I also made a post that would alter feedrates. I needed to slow plunging down on a part that had a lot of 'ribs' in it. All 3D with a ball EM, plunges were really hard on the tool, especially at high feedrates associated with 3D. I used post questions to give the programmer flexibility as to whether to use the feature or not, and how much reduction to apply to the feedrates. The post evaluates angle of descent as a percentage, and applies that percentage to the value that was entered by the programmer as a reduction factor. Programs came out long, but worked very well. Reduced tooling costs, while maximizing run times.

 

This may not be the answer for all situations, just one example of what can be done.