00:00:07,600
Adaptive clearing tool paths are commonly used for pocketing out large areas.
00:00:12,200
because of the way adaptive clearing calculates tool paths
00:00:15,566
its very efficient for odd shaped pockets with sharp corners.
00:00:20,066
adaptive clearing is the right tool path to use for removing large amounts of material quickly.
00:00:26,266
it can rough the outside to leave the boss standing,
00:00:29,500
Rough the inside of a closed boundary
00:00:32,233
and even clear out open pockets.
00:00:36,966
project maintenance is also an important part of consistency in your program tool paths.
00:00:42,200
so the first thing we're going to do is duplicate our existing adaptive tool path
00:00:46,866
and reuse it to machine additional features on the model.
00:00:51,566
the goal is to copy something we know works well and reuse it, only changing the parameters that might be different.
00:00:59,566
Another maintenance function is to give our tool paths meaningful names.
00:01:03,800
naming a tool path makes it easier to recognize,
00:01:06,966
organize and edit your operations.
00:01:10,000
so as an example let's say you spent some time getting this adaptive tool path exactly the way you want it.
00:01:15,900
if your next tool path will require a similar machining technique.
00:01:20,466
it's easier to make a duplicate of this tool path and then reselect the geometry or features to be machined,
00:01:27,400
to make a duplicate tool path simply mouse over the tool path you want a copy,
00:01:33,200
right click your mouse and from the pull down menu,
00:01:36,200
select duplicate.
00:01:39,500
now will have an exact duplicate of that tool path
00:01:43,466
changing the name of the tool path operation is a good practice for documentation purposes
00:01:48,700
if you have three and apt of clearing tool past you would want them named adaptive one
00:01:53,866
adaptive two adaptive three. you should give them a descriptive name
00:01:59,033
that helps document the machining process.
00:02:02,300
if you or someone else opened your file three months from now,
00:02:06,066
would they know what's happening with your tool paths.
00:02:08,933
so let's give these tool paths some descriptive names.
00:02:12,333
I want you to left click on the face tool path and then click again.
00:02:18,066
the name of the tool path is now highlighted so that we can edit that name. now we can type in a
00:02:24,266
short description of what this tool path does and we want to do this for all of our tool paths.
00:02:30,500
so for the face mill, say, face mill top
00:02:34,200
and press enter
00:02:35,633
for the adaptive tool path, again we'll click on it once and then again
00:02:41,933
and call it outside mill
00:02:44,533
and for our next adaptive tool path
00:02:48,266
we'll call this pocket mill. now we can modify our duplicate tool path to machine additional areas of the model.
00:02:55,566
double left click the pocketing tool path or you can right click and say edit.
00:03:01,466
the reason we made a duplicate is because the tool and most of the parameters will be the same
00:03:06,100
so we only need to modify the things that will be different
00:03:10,333
on the geometry tab
00:03:13,133
we could
00:03:14,500
de-select the current geometry
00:03:16,766
and now we can select the new edges that we want to machine
00:03:20,733
I want to pick the edge
00:03:22,466
of this open pocket here
00:03:25,166
and also the edge of this open pocket here.
00:03:29,100
on the Heights tab
00:03:31,566
we'll need to modify the bottom height.
00:03:34,466
our bottom height is from selected contour and our offset is .030", let's set that to zero
00:03:40,733
because we don't want to cut past the edge that we selected.
00:03:47,000
because that would gouge into this pocket.
00:03:49,800
if we press OK
00:03:51,800
we have an updated tool path to clear out those open pockets. if you examine this tool path,
00:03:57,100
you'll notice the tool stays close to the surface of the part. in most cases this is desirable
00:04:02,400
there are some cases where you may want a force the tool to retract during a cutting operation.
00:04:08,300
the parameters to do that are under the linking tab. so let's right click and edit this tool path and go to our are linking Tab.
00:04:17,900
the parameter that we want a change is
00:04:20,166
the maximum stay down value.
00:04:23,266
the larger the value of the more likely the tool will not take a full retract.
00:04:28,500
forcing the retract can be useful in parts with lots of steps pockets or ribs.
00:04:34,333
as an example let's change this value
00:04:37,200
to 1 inch
00:04:38,800
and OK this.
00:04:40,500
now because the distance from the end of one cut
00:04:44,566
back to the beginning of the next cut
00:04:46,900
is larger than the 1 inch value
00:04:50,766
it forces it to do our retract to move up and over to the next starting point.
00:04:55,733
feel free to try some different values in here and when you're done
00:05:03,066
set this back
00:05:04,966
to 2 1/2 inches.
00:05:09,766
now we need to cut some additional pockets in here on each end.
00:05:13,900
adding chains to an existing tool path is easy to do.
00:05:17,266
let's add more pockets to the tool path we just created.
00:05:22,066
open the pocketing tool path by going into edit.
00:05:26,666
and we'll go to our geometry Tab.
00:05:29,266
all we really need do is select the additional contours.
00:05:33,233
so come over here and select the bottom edge of this pocket,
00:05:38,000
and the bottom edge of this pocket. Make sure you're not picking the face.
00:05:42,433
because the face has a hole in it and it will try and avoid the hole. we only want to consider
00:05:50,500
the boundary edge of that pocket and OK that.
00:05:54,533
so if you look at this you can see it didn't do the pocket at all
00:05:59,566
The tool needs to enter into the cavity somehow
00:06:02,166
and the default is to use a helical entry into the part.
00:06:06,466
if you open the parameters again
00:06:11,200
and go to the linking tab,
00:06:13,400
down in the ramp section you'll see there's a helix a ramp diameter
00:06:17,733
and a minimum ramp diameter.
00:06:20,200
right now they're both set to the same value
00:06:23,266
I want you to set the minimum
00:06:25,633
to .120"
00:06:28,066
this tells it an acceptable range to calculate for the helix.
00:06:32,100
so no tool path was generated because the helix size was too large to fit into the cavity
00:06:37,633
by changing the minimum ramp to hammer to .120, fusion will calculate a size within that range
00:06:44,233
that will work to create a helical entry into the cavity
00:06:48,533
OK this.
00:06:50,633
now we can see that it's cut the open pockets
00:06:53,566
and our new pockets by ramping its way down to the depth