Adjust feedrates w/ swarf toolpath

[Smit]

Can anybody give me a tip on how to adjust feed rates in a swarf toolpath when the tool is fanning around a corner?

 

I have the feed rates box checked in the swarf milling parameter dialog box, and it outputs a feed rate of 30 on the entry, then changes to a feed rate of 10, but doesn't change the feed rate at all in the corners.

 

I'm using X4MU2.

 

Thanks!

[Josh T™]

Change at point?

 

Just thinking out loud. I'll look at it and get back to you.

[Smit]

There's no way to adjust the feedrates in the advanced 5 axis swarf toolpath?

[cobra95kev]

Smit,

Yes there is. Go to the advanced interface and go to the utility tab. Looks pretty cool but I have never tried it.

[Superman]

One of the faults with mastercam 5-axis swarf is that the plunge rate is also the entry/exit rate

 

Who in their right mind wants to have their plunge rate active when side cutting ??

 

The othe alternatives are to have plunge and XY feedrate the same, or use the toolpath editor and set a different rate before posting

[Jim at Gentex]

I'm not sure if there is a method to change the feedrate in mid-toolpath.

 

I use 5 axis swarf quite a bit for lens trimming.

It's difficult to tell where the trouble areas may be until you actually run the program on the machine.

 

I seldom see any issues, but if I do it's usually only in one or two small areas.

When that happens, I simply edit the nc file in the trouble spot and change the feedrate as needed.

 

edit:

On the swarf 5 axis parameters page (the page that shows wall following method) there is a 'fanning feedrate' box. I believe that is what you are looking for.

[Smit]

The part I'm trying to program is an internal rectangular shape, about 30 degrees slope, with radii in the corners. Big at the top and small at the bottom.

 

The feed rate is OK until the tool hits those internal corners and then when C axis starts rotating it really flies around the corners way too fast.

 

The machinists have been modifying the program to make it run and it does cut a nice part, but there should be a way to compensate for that fanning move around the corner.

[cobra95kev]

Do you not have the advanced multi-axis paths?

[mayday]

quote:

---

Yes there is. Go to the advanced interface and go to the utility tab. Looks pretty cool but I have never tried it.

---

Yup

I use it rolling airfoils, works good

[Smit]

quote:

---

Do you not have the advanced multi-axis paths?

---

I do. And it looks like it should work there but doesn't.

 

I have the feed/plunge rate set to the same feed. The feed in and out are at the plunge feed. It then kicks into a slower feed (which is OK as long as you can adjust it) but stays the same through the corners rather than reducing the feed rate again.

 

I must have something set wrong. I'll continue to play with it until it does what I need.

[gcode]

There are feedrate options in the mpgen post

If your post is based on that they may be still be there

 

[*]inv_fd_typ : 0 #Calculate feed location options

 

#0 - inverse feed at tip

#1 - min-max on flute length

#2 - tip to pivot on tool length

#3 - min-max on flute length to pivot on tool length

Typically the post is set at option 0

option 2 or 3 may give you better results for this particular toolpath

[Smit]

I'll give that a shot gcode.

 

Thanks for the info!

[Guest CNC Apps Guy 1]

What you REALLY want to do is level the velocity, which is not really possible unless machine kinematics are taken into consideration. As far as I can tell, MC has no way of doing this so I think #3 may be your best bet.

 

[shamelessplug] Man CAMplete sure handles this well...[/shamelessplug]

[Smit]

quote:

---

What you REALLY want to do is level the velocity,

---

Yes, I suppose that is what I REALLY want.

 

So you have my interest now. What is this CAMplete of which you speak?

 

Does it work with Mastercam or is it a different CAM software?