& Construction

Integrated BIM tools, including Revit, AutoCAD, and Civil 3D
& Manufacturing

Professional CAD/CAM tools built on Inventor and AutoCAD
Transcript
00:02
Finish Operation three of apart.
00:06
In this video we'll use to the adaptive to rough apart well rough and finish A two D.
00:10
Pocket will create drilling and tapping tool paths
00:13
and we'll use bore to finish a whole
00:17
infusion 3 60. Let's carry on with our engine case. Rh ready to program.
00:22
At this point we've created a two D. Adaptive to rough. Our pocket
00:27
has taken down the material to the very top of the boss.
00:29
But we've left 20.2 on the walls and the floor.
00:33
So now we need to go back with the same tool and we need
00:36
to finish the bottom of that pocket before we move on to the rest.
00:41
Because the two D. Adaptive tool path is a roughing tool path.
00:45
We're going to go back using a two D. Pocket tool path.
00:48
Both to the adaptive and pocket are roughing tool paths
00:52
to deep pocket does have a finishing option that allows us to machine both
00:55
the walls and the floor down to our final depth with higher precision.
00:60
So we're going to use two D. Pocket with the same tool.
01:03
Keeping in mind that the tools that we use generally will go in order.
01:07
So we don't have to initiate tool changes often and slow down our program.
01:12
So again, we want to make sure that our cutting feed rate is at 100 inches per minute.
01:16
And the geometry we're going to use is going to be the same geometry.
01:20
We want to select this bottom contour here.
01:22
However,
01:23
we are going to turn on stock contours and we do want to make
01:27
sure that our heights are set to a selection and not to our selected contour
01:32
from here. We're going to move on to our passes.
01:35
Now again, this is also a roughing tool path,
01:38
but we're going to turn off stock to leave.
01:41
We do want to think about if multiple depths are going to
01:44
be needed because we're not roughing out a bunch of material,
01:47
we're only taking a look at the .02 stock that was left on the floors and
01:52
the walls and the tool that we're using has an inch and a half cutting flu.
01:56
We can simply come in and finish the walls and the floor.
01:59
So again,
02:00
we don't really need to worry about coming in
02:03
and roughing or removing large amounts of material.
02:06
We do want to make sure that we enable a finishing pass and notice
02:10
that that opens up a few more options for us on the finishing pass,
02:14
we're going to leave the default .05 step over with one finishing pass.
02:19
Remember we left .02 on the walls and floor. So we're going to do this in a single pass,
02:24
I'm going to say okay, and allow the tool to come in
02:27
so you can see that it's clearing out not only the floor of the material,
02:30
but also the walls, it's moving all the way out to the side.
02:34
Now that we've used our half inch end mill to both rough
02:37
and finish all the way down to the top of this boss.
02:40
Let's go ahead and take a look at the smaller section based on the dimensions.
02:44
We don't have enough room to take a half inch tool in here.
02:47
If you want to verify this,
02:49
you can go to your last operation in this case are two D pocket.
02:53
We can go down to show hide tool,
02:55
we can show the tool and we can use this option to show tool on cursor.
03:00
When we use show tool on cursor,
03:02
we're able to rotate the model around and we can
03:05
see that it does not fit in between the space.
03:08
So this is an extremely helpful thing that we can do
03:10
to verify whether or not we can actually reuse that tool.
03:14
Of course we can measure and we'll know that there
03:16
is less than 3/8 of an inch inside of there.
03:18
So I'm going to go back and I'm going to hide the tool and the holder and
03:22
I'm going to move on to actually go through
03:25
and machinist with the quarter inch end mill.
03:27
So to remove this material in the bottom of the pocket,
03:30
we're once again going to use a two D adaptive clearing operation.
03:34
This time we need to select a new tool that we haven't used yet.
03:37
So in our intro to C and C library, we're going to select the quarter inch flute flat,
03:42
which is tool number five.
03:43
I want to select my aluminum roughing and select the tool When we look at this,
03:49
you can see that the spindle is set to 12,000 rpm.
03:53
The machine that we're using has a limit of about 7500.
03:56
So we need to reduce that and we need to make sure that we reduce it everywhere,
04:00
so 7500 rpm for both the ramp spindle speed and the default spindle speed.
04:06
Then we also need to think about the optimal load for this tool.
04:10
In this case, when we're using the quarter and gen mill,
04:12
the cutting feed rate is coming in at about 100 inches per minute.
04:17
I'm actually going to reduce this a little bit.
04:18
I'm gonna go down to 75" a minute and I'm gonna
04:21
do the same thing for the lead in and the lead out
04:25
notice that there is a higher ramp feed rate and
04:28
I'm going to allow the higher ramp feed rate,
04:30
but in this case I do want to make sure that the plunge feed rate is much smaller.
04:35
Now that we've adjusted those values, let's go to our geometry.
04:39
In this case we want to select the bottom
04:41
face because this is going to automatically detect the
04:44
island or the boss in the center and it's
04:46
only going to be machining this outside section.
04:48
So now that we have this selected,
04:50
we can also turn on stock contours if we want to
04:53
make sure that we do extend outside of that pocket,
04:57
let's go ahead and move this back into view.
04:59
When we turn off stock contours, you can see that it starts right here,
05:02
but we turn it on, it's going to allow the tool to enter from the outside.
05:07
Next we can't turn on rest machining.
05:09
However,
05:10
we're going to be using our heights to dictate where this is going to start and end.
05:14
So in the heights section, the top height is not going to be the stock top.
05:19
In this case,
05:20
what I want to do is use my selection and I
05:22
wanted to start cutting around the top of the boss.
05:26
Now if you are just starting out,
05:28
this is something you need to be very careful with because if you start programming
05:32
and adjusting your top heights to be below your actual top of your part,
05:36
you need to be very sure that the tool is
05:39
not going to make rapid movements and go through stock.
05:42
So we need to be very careful when we verify these tool paths
05:45
that it is staying within the confines of that area.
05:48
Now that we have this set, let's move on to our past section for roughing this cavity.
05:54
I want to take a look at this optimal load.
05:56
Now it's about 0.47 and I'm going to increase that 2.5 for this tool.
06:01
And when we take a look at the stock to leave 0.2 on both the wall on the floor,
06:06
that's going to be just fine.
06:08
I'm going to say okay and allow it to generate this. Notice that the tool is entering
06:14
and it's making that adaptive tool motion to clear everything out.
06:17
One other thing that we could do is we could dictate where
06:21
the tool is entering and this happens on the last tap.
06:24
So if we go back and edit this tool path and we go to our linking parameters,
06:28
we can use a pre drill position
06:30
to have the tool come into the part from the outside or from the center of a hole.
06:35
If we select entry positions and we select for
06:38
example a point on this wall and say okay,
06:41
it's going to automatically force the position where the tool is entering.
06:45
You'll notice that it recalculated our tool path and now the
06:48
tool is entering and exiting generally where we put it.
06:51
Now the exit happens based on where the tool path is finished.
06:55
But in some cases we can force the issue to dictate where it's going to start.
06:60
So in this case we now have adaptive lee cleared that bottom pocket.
07:04
But we left 0.2 on both the walls on the boss the outside and 0.2 on the floor.
07:10
So we're going to come back with a two D.
07:12
Pocket just like we did before using the same quarter inch
07:16
tool as well as the same rpm and feed rate.
07:19
And for our geometry, we want to make sure that we do select that same area.
07:23
I do want to note that there are options
07:25
for pocket recognition inside of these two D operations.
07:29
But when we're just getting started, understanding our selection,
07:32
whether it's a face or if we're selecting individual contours is
07:36
an important step in the process to understand where we're machining.
07:39
But I do want to mention that there are more advanced options that we can use.
07:43
In this case,
07:44
I am going to turn on the stock contours and again you can see that it does extend
07:49
this,
07:50
make sure that our tool is taking into account all the material
07:53
that may be left behind because we did adaptive lee clear everything.
07:57
The stock contour is not really going to add much for us in this case.
08:01
So I will be turning it off for this finishing step
08:04
For our heights.
08:06
We also have to think about where this tool path is starting for the last one.
08:10
When we did our adaptive clear, we started from the top of the boss.
08:14
If we happen to use the feed height as the top height plus .02,
08:19
that means the tool is going to feed all the way from this point,
08:22
all the way down at its reduced feed rate.
08:24
If we go back to our tool selection, you can see that it's leading in at 75" a minute.
08:31
So we do want to make sure that we adjust our heights.
08:33
But again, this is something we need to be extremely careful with.
08:37
We want to make sure that we are understanding where the tool is going to be
08:41
next in our passes. We do want to enable finish passes and disable stock to leave.
08:46
We want to think about the maximum step over 0.0 to five and we want
08:52
to think about our finished feed rate when we're looking at our step over value,
08:57
we should remember that there are actually two different step over values.
09:01
This 20.0 to 5 is for our finishing pass and there's
09:04
a maximum step over that's listed down here as 50.15.
09:08
This maximum step over here is going to account for the major movements of
09:13
the tool and the .025 will be used for our final finishing pass.
09:18
So I'm going to say okay, and allow it to generate this.
09:21
And again that it does know that it's starting from
09:24
outside because it does know that it's an open pocket.
09:27
So it's starting the tool path, entering and exiting from the outside,
09:31
moving its way in
09:32
finishing the floor as well as the outside and inside edges.
09:36
Now that we have these taken care of,
09:38
we can move on to taking care of all of the holes in the part.
09:42
There is going to be a specific order that we should think about this
09:46
and that's because we do need to do a couple of extra operations here.
09:50
We need to do some spot drilling as well as
09:53
some pre drilling and boring in the center here.
09:56
So let's get started and run quickly through
09:58
creating some drilling operations for the drilling operations.
10:02
Again.
10:03
We want to make sure that we are using our
10:05
spot drill and we're going to select tool number two,
10:08
which is our quarter inch spot drill.
10:11
We're going to select our positions and we're
10:13
going to start with the three large holes.
10:16
We need to use these because we don't want to
10:18
pre drill the same depth for the small holes.
10:21
So we're going to start by doing these.
10:22
And in the heights section we're going to use to champ for width.
10:26
It's not going to be able to account for that in the large hole,
10:29
but it will take these other passing holes down and we can say, okay,
10:34
since we have this tool active,
10:36
we're going to repeat the process creating drilling.
10:38
We're going to now select these holes here.
10:41
So I'm going to select these holes
10:45
and note that we want to use auto merge segments.
10:48
It's going to take up the champ for on top.
10:50
And then for the heights we want to use to champ for
10:53
width that's going to automatically account for the champ for for us,
10:56
we're going to leave all the rest of the settings the same and say, okay
11:01
Now we can create a drilling operation for the drilling operation.
11:04
We're going to use intro to C&C. And drill f. This is going to be a .257.
11:11
This drill bit is going to be used for this hole here.
11:15
This large center hole as well as this one.
11:18
We want to make sure that this goes all the way to the whole bottom and we're going
11:21
to allow the drill tip to go through bottom
11:23
just to ensure that we go all the way through
11:26
for this cycle. We're going to set this to chip breaking and we'll say, okay,
11:31
Next, what we're going to do is we're going to drill the smaller hole.
11:34
So once again, we're going to create a drilling operation.
11:37
But this time we're going to be using our .1-5 drill.
11:41
This is going to be a smaller drill bit tool number eight.
11:46
Next we're going to select our holes.
11:49
We're going to allow it to go all the way to the bottom.
11:51
But we are going to use the drill tip through bottom.
11:53
We talked about this earlier on the print because it's a flat bottom hole.
11:57
We either need to take a small end mill in there to finish
11:59
the flat bottom or we can drill the hole a little bit deeper,
12:03
assuming it's allowed based on the print.
12:05
Even though this is not a very deep hole,
12:07
I am still going to use the partial retract chip
12:10
breaking cycle just because it's a fairly small drill bit.
12:14
Next I am going to go ahead and create a bore in the center of this whole.
12:19
Now keep in mind that there are different order of
12:21
operations that we could take instead of using our spot drill
12:25
to take care of this chant for we could come back
12:27
and take care of it using our champ for mill.
12:29
We could also have chance for this whole before but
12:33
we're going to again just pick our order of operations,
12:35
noting that we can always move these things around later.
12:38
But now that we have this hole pre drilled,
12:41
what we want to do is we want to come back with a two D operation called bore.
12:46
We're going to select our quarter inch flat which is tool number five,
12:49
making sure that we are still fixed at spindle speed of
12:56
we're going to make sure that we are going all the way through the bottom of the hole.
13:00
So I'm going to add a small amount to the bottom of minus 0.5.
13:05
Remember when you're using the offset values,
13:07
it's going to be negative based on the Z orientation of our coordinate system.
13:12
When we have passes.
13:13
Note that we do have multiple passes and finished passes,
13:17
I do want to turn on a finishing pass
13:19
and I'm going to have it be a fairly small amount of .025 which is the default value.
13:24
We can also use multiple passes.
13:26
I'm going to do some roughing passes at .125 and I also
13:30
want to make sure that we are using a pre drill location.
13:34
So when we look at these various options, note that inside of here,
13:39
we've got all the various ramp angles, we've got multiple passes,
13:43
we've got finishing passes and so on.
13:45
But when we go to our geometry notice that inside of our
13:49
geometry we don't have the selected option for using a pre drill.
13:53
When we go to our first option here,
13:56
we're selecting the tool and setting the parameters.
13:59
So depending on the order of operations you might not have a pre drill
14:04
or an entry position but when we're using circular tool paths like boar,
14:08
we can always use the lead to center option.
14:11
Now as we turn this on and off,
14:13
you can see all these yellow lead movements move directly to the center.
14:17
So if you are using a board tool path and you have pre drilled it,
14:20
it is important that we think about these options and we do move the tool to the center
14:26
now that we've machined essentially everything,
14:29
we can go back using R two D champ for.
14:31
We can select an appropriate chant for tool and
14:34
again we're going to select tool number three,
14:37
this is going to be our quarter inch champ for mill
14:40
and then we're going to move on to our geometry.
14:43
We want to chant for the entire outside and we also want to come
14:46
back in and take care of these holes when we're using the champ formal,
14:50
these values are going to be set based on the champ for width,
14:53
the tip offset and the chance for clearance.
14:56
So we're going to use 0.1 for the champ for width,
14:59
point oh five for the tip offset and 50.1 for the tip clearance will say okay,
15:06
allow it to deeper all those.
15:08
And now we've finished off op three.
15:11
Do note that we do have a warning on the board tool path.
15:14
It tells us that some passes were disregarded,
15:17
reduce the tool size or decrease the step over amount.
15:20
It's a good idea for us to double check these warnings and
15:23
make any adjustments needed because we're not removing that much material,
15:27
we can go back to our passes and do just a single roughing step over,
15:31
allow it to regenerate the tool path and we can see now we no longer have the warning
15:36
essentially we had an extra path that wasn't producing any tool path cuts
15:41
Now that we have this let's go back to our op three view and
15:45
let's make sure that we save this before we move on to the next step
00:02
Finish Operation three of apart.
00:06
In this video we'll use to the adaptive to rough apart well rough and finish A two D.
00:10
Pocket will create drilling and tapping tool paths
00:13
and we'll use bore to finish a whole
00:17
infusion 3 60. Let's carry on with our engine case. Rh ready to program.
00:22
At this point we've created a two D. Adaptive to rough. Our pocket
00:27
has taken down the material to the very top of the boss.
00:29
But we've left 20.2 on the walls and the floor.
00:33
So now we need to go back with the same tool and we need
00:36
to finish the bottom of that pocket before we move on to the rest.
00:41
Because the two D. Adaptive tool path is a roughing tool path.
00:45
We're going to go back using a two D. Pocket tool path.
00:48
Both to the adaptive and pocket are roughing tool paths
00:52
to deep pocket does have a finishing option that allows us to machine both
00:55
the walls and the floor down to our final depth with higher precision.
00:60
So we're going to use two D. Pocket with the same tool.
01:03
Keeping in mind that the tools that we use generally will go in order.
01:07
So we don't have to initiate tool changes often and slow down our program.
01:12
So again, we want to make sure that our cutting feed rate is at 100 inches per minute.
01:16
And the geometry we're going to use is going to be the same geometry.
01:20
We want to select this bottom contour here.
01:22
However,
01:23
we are going to turn on stock contours and we do want to make
01:27
sure that our heights are set to a selection and not to our selected contour
01:32
from here. We're going to move on to our passes.
01:35
Now again, this is also a roughing tool path,
01:38
but we're going to turn off stock to leave.
01:41
We do want to think about if multiple depths are going to
01:44
be needed because we're not roughing out a bunch of material,
01:47
we're only taking a look at the .02 stock that was left on the floors and
01:52
the walls and the tool that we're using has an inch and a half cutting flu.
01:56
We can simply come in and finish the walls and the floor.
01:59
So again,
02:00
we don't really need to worry about coming in
02:03
and roughing or removing large amounts of material.
02:06
We do want to make sure that we enable a finishing pass and notice
02:10
that that opens up a few more options for us on the finishing pass,
02:14
we're going to leave the default .05 step over with one finishing pass.
02:19
Remember we left .02 on the walls and floor. So we're going to do this in a single pass,
02:24
I'm going to say okay, and allow the tool to come in
02:27
so you can see that it's clearing out not only the floor of the material,
02:30
but also the walls, it's moving all the way out to the side.
02:34
Now that we've used our half inch end mill to both rough
02:37
and finish all the way down to the top of this boss.
02:40
Let's go ahead and take a look at the smaller section based on the dimensions.
02:44
We don't have enough room to take a half inch tool in here.
02:47
If you want to verify this,
02:49
you can go to your last operation in this case are two D pocket.
02:53
We can go down to show hide tool,
02:55
we can show the tool and we can use this option to show tool on cursor.
03:00
When we use show tool on cursor,
03:02
we're able to rotate the model around and we can
03:05
see that it does not fit in between the space.
03:08
So this is an extremely helpful thing that we can do
03:10
to verify whether or not we can actually reuse that tool.
03:14
Of course we can measure and we'll know that there
03:16
is less than 3/8 of an inch inside of there.
03:18
So I'm going to go back and I'm going to hide the tool and the holder and
03:22
I'm going to move on to actually go through
03:25
and machinist with the quarter inch end mill.
03:27
So to remove this material in the bottom of the pocket,
03:30
we're once again going to use a two D adaptive clearing operation.
03:34
This time we need to select a new tool that we haven't used yet.
03:37
So in our intro to C and C library, we're going to select the quarter inch flute flat,
03:42
which is tool number five.
03:43
I want to select my aluminum roughing and select the tool When we look at this,
03:49
you can see that the spindle is set to 12,000 rpm.
03:53
The machine that we're using has a limit of about 7500.
03:56
So we need to reduce that and we need to make sure that we reduce it everywhere,
04:00
so 7500 rpm for both the ramp spindle speed and the default spindle speed.
04:06
Then we also need to think about the optimal load for this tool.
04:10
In this case, when we're using the quarter and gen mill,
04:12
the cutting feed rate is coming in at about 100 inches per minute.
04:17
I'm actually going to reduce this a little bit.
04:18
I'm gonna go down to 75" a minute and I'm gonna
04:21
do the same thing for the lead in and the lead out
04:25
notice that there is a higher ramp feed rate and
04:28
I'm going to allow the higher ramp feed rate,
04:30
but in this case I do want to make sure that the plunge feed rate is much smaller.
04:35
Now that we've adjusted those values, let's go to our geometry.
04:39
In this case we want to select the bottom
04:41
face because this is going to automatically detect the
04:44
island or the boss in the center and it's
04:46
only going to be machining this outside section.
04:48
So now that we have this selected,
04:50
we can also turn on stock contours if we want to
04:53
make sure that we do extend outside of that pocket,
04:57
let's go ahead and move this back into view.
04:59
When we turn off stock contours, you can see that it starts right here,
05:02
but we turn it on, it's going to allow the tool to enter from the outside.
05:07
Next we can't turn on rest machining.
05:09
However,
05:10
we're going to be using our heights to dictate where this is going to start and end.
05:14
So in the heights section, the top height is not going to be the stock top.
05:19
In this case,
05:20
what I want to do is use my selection and I
05:22
wanted to start cutting around the top of the boss.
05:26
Now if you are just starting out,
05:28
this is something you need to be very careful with because if you start programming
05:32
and adjusting your top heights to be below your actual top of your part,
05:36
you need to be very sure that the tool is
05:39
not going to make rapid movements and go through stock.
05:42
So we need to be very careful when we verify these tool paths
05:45
that it is staying within the confines of that area.
05:48
Now that we have this set, let's move on to our past section for roughing this cavity.
05:54
I want to take a look at this optimal load.
05:56
Now it's about 0.47 and I'm going to increase that 2.5 for this tool.
06:01
And when we take a look at the stock to leave 0.2 on both the wall on the floor,
06:06
that's going to be just fine.
06:08
I'm going to say okay and allow it to generate this. Notice that the tool is entering
06:14
and it's making that adaptive tool motion to clear everything out.
06:17
One other thing that we could do is we could dictate where
06:21
the tool is entering and this happens on the last tap.
06:24
So if we go back and edit this tool path and we go to our linking parameters,
06:28
we can use a pre drill position
06:30
to have the tool come into the part from the outside or from the center of a hole.
06:35
If we select entry positions and we select for
06:38
example a point on this wall and say okay,
06:41
it's going to automatically force the position where the tool is entering.
06:45
You'll notice that it recalculated our tool path and now the
06:48
tool is entering and exiting generally where we put it.
06:51
Now the exit happens based on where the tool path is finished.
06:55
But in some cases we can force the issue to dictate where it's going to start.
06:60
So in this case we now have adaptive lee cleared that bottom pocket.
07:04
But we left 0.2 on both the walls on the boss the outside and 0.2 on the floor.
07:10
So we're going to come back with a two D.
07:12
Pocket just like we did before using the same quarter inch
07:16
tool as well as the same rpm and feed rate.
07:19
And for our geometry, we want to make sure that we do select that same area.
07:23
I do want to note that there are options
07:25
for pocket recognition inside of these two D operations.
07:29
But when we're just getting started, understanding our selection,
07:32
whether it's a face or if we're selecting individual contours is
07:36
an important step in the process to understand where we're machining.
07:39
But I do want to mention that there are more advanced options that we can use.
07:43
In this case,
07:44
I am going to turn on the stock contours and again you can see that it does extend
07:49
this,
07:50
make sure that our tool is taking into account all the material
07:53
that may be left behind because we did adaptive lee clear everything.
07:57
The stock contour is not really going to add much for us in this case.
08:01
So I will be turning it off for this finishing step
08:04
For our heights.
08:06
We also have to think about where this tool path is starting for the last one.
08:10
When we did our adaptive clear, we started from the top of the boss.
08:14
If we happen to use the feed height as the top height plus .02,
08:19
that means the tool is going to feed all the way from this point,
08:22
all the way down at its reduced feed rate.
08:24
If we go back to our tool selection, you can see that it's leading in at 75" a minute.
08:31
So we do want to make sure that we adjust our heights.
08:33
But again, this is something we need to be extremely careful with.
08:37
We want to make sure that we are understanding where the tool is going to be
08:41
next in our passes. We do want to enable finish passes and disable stock to leave.
08:46
We want to think about the maximum step over 0.0 to five and we want
08:52
to think about our finished feed rate when we're looking at our step over value,
08:57
we should remember that there are actually two different step over values.
09:01
This 20.0 to 5 is for our finishing pass and there's
09:04
a maximum step over that's listed down here as 50.15.
09:08
This maximum step over here is going to account for the major movements of
09:13
the tool and the .025 will be used for our final finishing pass.
09:18
So I'm going to say okay, and allow it to generate this.
09:21
And again that it does know that it's starting from
09:24
outside because it does know that it's an open pocket.
09:27
So it's starting the tool path, entering and exiting from the outside,
09:31
moving its way in
09:32
finishing the floor as well as the outside and inside edges.
09:36
Now that we have these taken care of,
09:38
we can move on to taking care of all of the holes in the part.
09:42
There is going to be a specific order that we should think about this
09:46
and that's because we do need to do a couple of extra operations here.
09:50
We need to do some spot drilling as well as
09:53
some pre drilling and boring in the center here.
09:56
So let's get started and run quickly through
09:58
creating some drilling operations for the drilling operations.
10:02
Again.
10:03
We want to make sure that we are using our
10:05
spot drill and we're going to select tool number two,
10:08
which is our quarter inch spot drill.
10:11
We're going to select our positions and we're
10:13
going to start with the three large holes.
10:16
We need to use these because we don't want to
10:18
pre drill the same depth for the small holes.
10:21
So we're going to start by doing these.
10:22
And in the heights section we're going to use to champ for width.
10:26
It's not going to be able to account for that in the large hole,
10:29
but it will take these other passing holes down and we can say, okay,
10:34
since we have this tool active,
10:36
we're going to repeat the process creating drilling.
10:38
We're going to now select these holes here.
10:41
So I'm going to select these holes
10:45
and note that we want to use auto merge segments.
10:48
It's going to take up the champ for on top.
10:50
And then for the heights we want to use to champ for
10:53
width that's going to automatically account for the champ for for us,
10:56
we're going to leave all the rest of the settings the same and say, okay
11:01
Now we can create a drilling operation for the drilling operation.
11:04
We're going to use intro to C&C. And drill f. This is going to be a .257.
11:11
This drill bit is going to be used for this hole here.
11:15
This large center hole as well as this one.
11:18
We want to make sure that this goes all the way to the whole bottom and we're going
11:21
to allow the drill tip to go through bottom
11:23
just to ensure that we go all the way through
11:26
for this cycle. We're going to set this to chip breaking and we'll say, okay,
11:31
Next, what we're going to do is we're going to drill the smaller hole.
11:34
So once again, we're going to create a drilling operation.
11:37
But this time we're going to be using our .1-5 drill.
11:41
This is going to be a smaller drill bit tool number eight.
11:46
Next we're going to select our holes.
11:49
We're going to allow it to go all the way to the bottom.
11:51
But we are going to use the drill tip through bottom.
11:53
We talked about this earlier on the print because it's a flat bottom hole.
11:57
We either need to take a small end mill in there to finish
11:59
the flat bottom or we can drill the hole a little bit deeper,
12:03
assuming it's allowed based on the print.
12:05
Even though this is not a very deep hole,
12:07
I am still going to use the partial retract chip
12:10
breaking cycle just because it's a fairly small drill bit.
12:14
Next I am going to go ahead and create a bore in the center of this whole.
12:19
Now keep in mind that there are different order of
12:21
operations that we could take instead of using our spot drill
12:25
to take care of this chant for we could come back
12:27
and take care of it using our champ for mill.
12:29
We could also have chance for this whole before but
12:33
we're going to again just pick our order of operations,
12:35
noting that we can always move these things around later.
12:38
But now that we have this hole pre drilled,
12:41
what we want to do is we want to come back with a two D operation called bore.
12:46
We're going to select our quarter inch flat which is tool number five,
12:49
making sure that we are still fixed at spindle speed of
12:56
we're going to make sure that we are going all the way through the bottom of the hole.
13:00
So I'm going to add a small amount to the bottom of minus 0.5.
13:05
Remember when you're using the offset values,
13:07
it's going to be negative based on the Z orientation of our coordinate system.
13:12
When we have passes.
13:13
Note that we do have multiple passes and finished passes,
13:17
I do want to turn on a finishing pass
13:19
and I'm going to have it be a fairly small amount of .025 which is the default value.
13:24
We can also use multiple passes.
13:26
I'm going to do some roughing passes at .125 and I also
13:30
want to make sure that we are using a pre drill location.
13:34
So when we look at these various options, note that inside of here,
13:39
we've got all the various ramp angles, we've got multiple passes,
13:43
we've got finishing passes and so on.
13:45
But when we go to our geometry notice that inside of our
13:49
geometry we don't have the selected option for using a pre drill.
13:53
When we go to our first option here,
13:56
we're selecting the tool and setting the parameters.
13:59
So depending on the order of operations you might not have a pre drill
14:04
or an entry position but when we're using circular tool paths like boar,
14:08
we can always use the lead to center option.
14:11
Now as we turn this on and off,
14:13
you can see all these yellow lead movements move directly to the center.
14:17
So if you are using a board tool path and you have pre drilled it,
14:20
it is important that we think about these options and we do move the tool to the center
14:26
now that we've machined essentially everything,
14:29
we can go back using R two D champ for.
14:31
We can select an appropriate chant for tool and
14:34
again we're going to select tool number three,
14:37
this is going to be our quarter inch champ for mill
14:40
and then we're going to move on to our geometry.
14:43
We want to chant for the entire outside and we also want to come
14:46
back in and take care of these holes when we're using the champ formal,
14:50
these values are going to be set based on the champ for width,
14:53
the tip offset and the chance for clearance.
14:56
So we're going to use 0.1 for the champ for width,
14:59
point oh five for the tip offset and 50.1 for the tip clearance will say okay,
15:06
allow it to deeper all those.
15:08
And now we've finished off op three.
15:11
Do note that we do have a warning on the board tool path.
15:14
It tells us that some passes were disregarded,
15:17
reduce the tool size or decrease the step over amount.
15:20
It's a good idea for us to double check these warnings and
15:23
make any adjustments needed because we're not removing that much material,
15:27
we can go back to our passes and do just a single roughing step over,
15:31
allow it to regenerate the tool path and we can see now we no longer have the warning
15:36
essentially we had an extra path that wasn't producing any tool path cuts
15:41
Now that we have this let's go back to our op three view and
15:45
let's make sure that we save this before we move on to the next step
Step-by-step guide