reduce feed in corners

[Smrkoul]

Hi,

can X3 reduce feed when tool is approaching to corner (in pocket toolpath, 2D contour etc.) I cant find this option anywhere. Please help, thanks.

[Robert Bell]

You can right click in operations mgr window, look for edit option, I think you will be looking for "change at point". You have the ability to change feed rates and rpm etc at any point on toolpath. Can't be more specific, my hasp is at work. Been a while since I used that option.

HTH

[Smrkoul]

thanx, i found it. But it is quite slow to edit all radius in toolpath point by point. Is there any faster way? global setting?...

And if i am machining pocket with R4 in a corner and have tool diameter 8, than toolpath has sharp corners. So is it possilbe to reduce feed before tool approach corner but straight lines go with full feed?

[3R!< W3NG3R]

Try the high feed option. its beside the G1 in the ops manager. looks like an and mill with an arrow pointing to the right. I can't tell you how to use it though, as I haven't played with it enough to get it to work right.

 

HTH

[mike_f]

I added this code to my posts ...

code:

---

  pcirout1        #Output to NC of circular interpolation

pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,

pxout, pyout, pzout, pcout, parc,

 

(from here)

 

[

if iout,

[if iout <mr2$ & iout >-mr2$ ,feed = feed*mr1$]

else,

if jout,

[if jout <mr2$ & jout >-mr2$ ,feed = feed*mr1$]

],

 

(to here)

 

feed, strcantext, scoolant, e$

---

to use misc. reals to change the feeds during circle output if my I or J values fall above or below the value I specify in mr2.

ex: if I want to reduce my feed by 50% whenever an I or J value falls below .03 , I input .03 into mr2 and .5 into mr1 , the feeds are reduced for the G02 and G03 blocks that have I's or J's less than .03 and then return to normal for G01. this can also be used to increase feeds on outside radii by inputing a larger number than one in mr1, a value of 1.5 would increase your feed by 50%.

 

HTH

mike

[bigjohn]

Very interesting sir.

 

 

John

[Matthew Hajicek - Singularity]

I suppose one could expand on this by having code that pays attention to which way you're comping to see if an arc in inside or outside, and then change the feedrate based on a function of the radius.

[Salt4cad]

This is the best I believe cut feed by 75%

set misc setting to 1 for contour path

pcirout #Output to NC of circular interpolation

if mi10$ =1, pstevesfeed

pcan1, pbld, n$, `sgfeed, sgplane, sgcode, sgabsinc, pccdia,

pxout, pyout, pzout, pcout, parc, feed, strcantext, scoolant, e$

feed = sav_fdd

 

pstevesfeed

sav_fdd = feed

feed = feed/4

[mike_f]

the reason I like using I & J values to reduce/increase my feed is that , for example: if I'm using a .5 end mill and I have 6 radii in a pocket, 3 of them are .27 and 2 of them are 1.5, well a .5 end mill cutting a .27 radius greatly increases the radial chip load on my tool and yet the 1.5 rad might as well be a straight line cut, I would set my misc. real to change my feed for any block with an I or J between .025 and -.025, this way only the feed in the small radii is affected helping me to eliminate tool deflection in those areas. In my lathe posts I use I & K. works the same way.

[Brian Duprey]

Regarding using the Highfeed option... This will slow the tool down in the corners. you have to make sure that your 'Machine Dynamics' are set up correctly in the 'General Machine Perametes' section of your Machine Def.

When you go to High Feed leave it set to finishing only and it will use the info in 'Machine Dynamics' to slow down the tool

 

----------------

Brian

[chipman]

I have not tried this but there is a dialog box in you Machine Group Properties Tool Settings tab called "adjust feed on arc move"

 

According to the help page:

 

"Adjusts the current linear feed rate to fit arc geometry. The feed rate change occurs at the start point of the arc. the adjusted feed rate cannot exceed the linear feed rate and cannot fall below the minimum arc feed rate.

[Matthew Hajicek - Singularity]

I've used that occasionally, but what I don't like about it is that it's either on or off for your whole machine group. I've requested that it be moved to the individual operations.

[Justin Beebe at Folsom Tool]

Someone on the forum said they can get "adjust feed on arc moves" to work only on certain toolpaths by doing the following:

 

1. turn on adjust feed on arcs moves

2. regen your toolpaths

3. lock the toolpaths you want it to

work on

4. turn off adjust feed on arc moves

5. regen your toolpaths

 

It won't turn it off on the locked toolpaths.

 

I have not tried this but I'm curious to see if it works.

[spade117]

The steps Justin posted work. I've done it in the past myself that way.