Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Advanced Multiaxis question


WesC
 Share

Recommended Posts

Hello all,

 

When I use the 5 axis swarf function, the speed seems to be relative to the tip of the tool. I am sure that in most cases that is what I should want.

 

In this example, the top part of the cutter is going much faster than I would like. It is leaving a pretty rough finish. Is there anyway to make the speed more relevant to the center of my cut?

 

 

<a  href=5AXISTEST.jpg' alt='5AXISTEST.jpg'>

Link to comment
Share on other sites

This can be affected by a couple of things.

Is your output tool tip with the control doing the comp

or pivot point with you posting a gage length..

 

I'm guessing you're running pivot point/gage length

 

If you look in your post, there are a couple of switches for feedrate.

 

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

 

You probably have it set a 0

Try setting it to 1 or 2

When its set at 1, the flute length definition

will affect feedrate..

Set at 2, the tool length will will effect it.

 

It would be nice to be able to change this on the fly as some cuts need feedrate applied at the tip

and others along the flute.

Link to comment
Share on other sites

quote:

If you look in your post, there are a couple of switches for feedrate.

 

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

 

You probably have it set a 0

Try setting it to 1 or 2

When its set at 1, the flute length definition

will affect feedrate..

Set at 2, the tool length will will effect it.


With a table/table setup, I did not found any difference when I played with these a while back.....no matter how I set them, the feedrates stayed the same.

 

quote:

It would be nice to be able to change this on the fly as some cuts need feedrate applied at the tip

and others along the flute.

This is one thing I have not had to play with (using CamPlete), but there appears to be a way to do this (or something close to it) with advanced multiaxis. Under the "utility" tab there is a "Feed rate advanced control" tab that lets you adjust your feedrate according to the surface curvature. Might take a bit of playing with to get things right....but might be worth a try.

Link to comment
Share on other sites

quote:

With a table/table setup, I did not found any difference when I played with these a while back.....no matter how I set them, the feedrates stayed the same.

they shouldn't have any effect on a table/table setup.. the velocity of the tool is constant along its entire length .. it doesn't matter if the tool is 1" long or 6"

 

On a head/head setup, the tip of the tool can be stationary while the flutes are moving quite rapidly. Wesc's sketch is a perfect example of this.

Sweeping around the corners of that slot, the tool tip is hardly moving yet the flank of the tool is probably moving too fast.

Link to comment
Share on other sites
Guest CNC Apps Guy 1

JMC, to adjust the velocity in CAMplete, you select the 4/5 Axis cut you want to affect the velocity for, right click on it and select "Optimize". Go to the Velocity (IIRC) tab and set how you want to level the velocity.

 

HTH

Link to comment
Share on other sites

James,

 

The thing I like about CamPlete & parts like this one is when you level the relative velocity, you can specify a max feedrate....so when you go around the corner, it is not going crazy fast. I had only looked into the "Feedrate advanced control" thing the other day & it looks to have similar functionality as far as being able to slow down a feedrate when going around a tight corner....minus the realtime simulation so y0u can get an idea as to how fast the machine is moving.

Link to comment
Share on other sites
Guest CNC Apps Guy 1

CAMplete kicks @$$!!! I've been playing with V4.5 and the material removal simulation. It's a bit on the slow side but I have no doubt they will improve the speed. The guys at CAMplete are some of the most responsive Software Engineers I've ever even heard of. There has been two occasins where they got me a patch the same day I uncovered an issue.

Link to comment
Share on other sites
  • 9 years later...

Sorry for digging up an old thread, but I am having the same issue except with a Heidenhain post I cannot find the variables that GCode mentioned. Does anyone know what to look for in the post for Heidenhain?

Link to comment
Share on other sites
6 minutes ago, BCW said:

Sorry for digging up an old thread, but I am having the same issue except with a Heidenhain post I cannot find the variables that GCode mentioned. Does anyone know what to look for in the post for Heidenhain?

Do a text search of your post for this

 

"inv_fd_typ "

 

If this doesn't come up

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

 

you probably have a post that was purchased and the meat of the post is

in the encrypted PSB file.

If that is the case, you will have to go to the post developer for edits 

 

Link to comment
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • Recently Browsing   0 members

    • No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us

×
×
  • Create New...