|
Well now, would you look at that little question
number 47 now? It does seem to do what I was attempting to do thru the
.tmp file....... with one exception.
I was thinking that this adjustment should ONLY be
made for finish cutting passes, especialy if you are milling a rectangular bar
to round ends, the last thing you want as you take away the heaviest corner is
to speed up.
I will fool around some with the .tmp file, and
link it to only finish cutting in the .jof, and see how it works.
All replies are still welcome though.
thanks again
Jon
----- Original Message -----
Sent: Tuesday, January 30, 2001 8:45
AM
Subject: Re: [mfg-smartcam] Feed rate
adjustments?
It seems to me that you have all the information you need to do
the work in the
.TMP file, I am just speaking in theory here because I am a
little short on
time. That said, in your ARC section you
can
capture the original feedrate and store it in a
variable
capture the tool diameter from the job
plan
capture the programmed radius
set a
variable equal to programmed radius divided by the feature radius
(this
would be the programmed radius+the tool radius)
evaluate the
variable to see if it is <.5
If the variable is <.5 set
the variable = to the feedrate * variable
then use the
variable in place of the #feed word
then reset the #feed to
force the next line or profile section to output a
feed
And this may
all be possible from the .SMF file. . .it seems there is a question
there
about slowing down for arcs.
Sorry I don't have time to give you the
specific code or commands.
David
"Jon Baker"
<[EMAIL PROTECTED]> on 01/30/2001 11:23:59 AM
To:
[EMAIL PROTECTED]
cc: (bcc: Dave
Hayden/elliott)
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
|
