I never try to update the system variables like #FEED. Instead, I use avariable like #FEED_MOD. Then I set #FEED_MOD=(some value or calculation) The string will look similar to this
< #MOV>< X#XPOS>< Z#ZPOS> I#XCTR K#ZCTR< F#FEED_MOD>
As I recall if you are going to use a variable name like #FEED_MOD, you need to
declare the variable in a @DECLARE section at the beginning of the file.
for example:
@DECLARE
#INT #homeflag//variable used to indicate tool is at home value of 1 = at home
***#INT = variable type Integer
#DEC #FEED_MOD//variable used to output modified or calculated feed rates
***#DEC = variable type Decimal
David
"Nix, Dan" <[EMAIL PROTECTED]> on 01/30/2001 01:00:02 PM
To: [EMAIL PROTECTED]
cc: (bcc: Dave Hayden/elliott)
Subject: RE: [mfg-smartcam] Feed rate adjustments?
Here is an Excel spread sheet I developed to determine the proper chip load
for cutting radii (internal).
Basically its Part diameter - Cutter diameter X Feedrate
Part diameter
I tried doing this through the template file, but what happened to me was
this, when my cutter radius was very close to the radius I was trying to
generate, it would reduce the feedrate to such a low number, it would almost
be a dwell in the corner. This caused chatter and other undesirable things.
I just gave up on the idea and now adjust the feedrate with a #FEED=X.XXX
user command.
-----Original Message-----
From: Jon Baker [mailto:[EMAIL PROTECTED]]
Sent: Tuesday, January 30, 2001 8:24 AM
To: [EMAIL PROTECTED]
Subject: [mfg-smartcam] Feed rate adjustments?
Hey group, I have a question for the masses.
Whenever I machine a slot, the sides tend to be on size, but the length
is short. So I have routinely slowed down the cutter feed rate at the end
of the slot to compensate for the short programmed path, as compare to the
feature.
ie) Mill a 1/2 slot, full end radii, with a 3/8 end mill, the programmed
path end radius is only .0625 when programming to tool center. I never
really had a formula for the amount to reduce the feed rate, but have seen
it now explained as the cutter path rad. divided by the feature radius,
times the feedrate.
ie) .0625/.25=.25 factor. .25 x 20 ipm=5ipm for end radius, then back
up to 20ipm for the straight away, just like nascar.
OK, fine, this seems logical enough for a formula, tho if anyone else has a
better one, I would love to hear it.
NOW THE QUESTION....
Is there a way to make smartcam do this calculation for me whenever the
factor value is .... say, under .50?
This would eliminate all the feed rate changes and returns in the shape
file, making it just simply the geometry to program.
If not a template section, what about a macro to adjust feed rate down a
percentage, then return it, from picking only a single element?
This isn't the most pressing issue, just trying to further my limited
intelect (sp) dang, as if I have much.
Thanks group
Jon Baker
|
Here
is an Excel spread sheet I developed to determine the proper chip load for
cutting radii (internal).
Basically its Part diameter - Cutter
diameter X Feedrate
Part diameter
I
tried doing this through the template file, but what happened to me was this,
when my cutter radius was very close to the radius I was trying to generate, it
would reduce the feedrate to such a low number, it would almost be a dwell in
the corner. This caused chatter and other undesirable things. I just gave up on
the idea and now adjust the feedrate with a #FEED=X.XXX user
command.
|
CUT-CALC.XLS
Description: Microsoft Excel 5.0
