[♪ Music Playing ♪] Hey everybody, it's Alex with Engineering
Applied! In this video, we're going to be
accelerating your career, hobby, or business
with this overview of the available Extrude tools in Autodesk Inventor.
If you're looking for a specific function, check the description for time
stamps. If you don't find what you're looking
for in this video, make sure you check out the other videos within the Autodesk
Inventor Series. Also, don't forget to like this video,
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Let's get started! Okay, so to aid us in this overview of the
extrude functions in Autodesk Inventor, we're actually going to be developing a
mounting fixture for an electrodynamic shaker and if you don't know what that
is don't worry. What it essentially does, is it acts like
a speaker. So think of a really big speaker
except the main objective isn't to create sound, it's to create
a vibration profile meant to test various parts that you put on it. So
in my case, I used it in the aviation industry to test electromechanical
components before they go into an airplane to make sure they could perform
under the stress of various vibration profiles.
So, in this case, what you're looking at here
is we've got a large square plate and on the four corners we have our mounting
interface between this plate and the actual
shaker itself. So this could take the form of a direct mount to the
electrodynamic shaker itself or to a slip table.
And if you're not sure what those are, let me know if you'd like me to do a
video on those specifically because I'd be happy to
shed some light on what that is for you. But, if we look closer at the plate,
we have a grid of singularly sized holes. So this is to
accommodate a 10-32 fastener, and they are spaced one inch apart. So
our objective here is to create a neutral mounting area for
whatever parts that we want to test so that we don't have to create a bunch of
these parts over and over again to match specific
parts that we want to test on our vibe fixture.
And this is really important for you engineers out there that might be doing
this because you don't want to waste a lot of money and machining time and down
time creating new fixtures, and you know, creating new designs for no reason if
you can help it. So this is the practical case I wanted to give you,
and I know this is sort of a roundabout way of getting to the extrude tools but
I think it's really important that we relate
real-life uses for these lessons because I want you to
learn and I want this information to actually stick so that you can
improve your quality of work whether it's in your career or whatever
else it is that you're doing. So, let's go ahead and get started here. What
we'll do is we'll create a new part file. So I've
already got one open here, and we'll just start a new sketch
because we've got to start our background for the actual square profile
for the plate. Okay so I went ahead and drew
up a 16 inch square shape which is going to act as our
profile for the plate itself. So we've got that
drawn up, now what do we do? So, like I always say in my videos,
you want to make sure that your sketches are fully defined. So in this case, we
know our sketch is fully defined because the profile
is all in the color black and if I were to go grab any of these sides, it's not going anywhere, it's not going to move.
And you'll also notice down here it says, "fully constrained". So after we've
done a good job of making our sketches fully constrained, we're going to go
ahead and jump out by either clicking "finish sketch"
here or we can just right click and go to finish 2D sketch here. And
now that we're out of our sketch, we're going to make sure we're in the 3D model
tab and we just click extrude. Now, you'll notice that it'll infer
the profile that you want to extrude. In this case, we only have the one square so
it knows, "hey this must be what this user wants to extrude". So
we will start looking at some of our options in here and as we progress
through this lesson, I'll make sure that we hit all of these options while
relating it to this practical use. So, at the top here we have our extrude
properties. You can "X" out of this but that'll cancel
out of the extrude command so we'll just actually go back in there.
Next, you have this little plus arrow. So this will add
various tabs to this extrude window so if you're using iLogic commands or
anything like that, or you could go into your favorites, so
you have a bunch of your content center resources in here
and whatnot. And at the end here, if you click this, we
have a few options for how the extrude behaves.
This first option here essentially says, "hey, when you have your sketch
that you're creating an extrude off of, and you press this little plus sign to
apply this extrude but also immediately start the next command,
it will keep that sketch visible or if you uncheck it it will not". So if I
uncheck this, or actually let's leave it checked first.
So if I check that, it leaves that sketch visible and it
automatically starts a secondary extrude without me having to go in and out of
the window. Now, if I was to go back and redo that,
and just go up here, uncheck that, and then if I hit the plus sign,
it exits out of the extrude and it leaves the command alone. So that's what
the difference in that command does. So we'll just undo that once again, we'll
go back to extrude. And let's take a look here. So we have
our "hide preset". So when you check that, it hides this
little preset option selector; we'll get to that in
just a moment. Okay, we also have the "single ENTER to finish command". So what
this allows us to do, is it allows us to, let's say for example, we wanted to
change this distance. So let's change it to 1.5,
and if I press enter here it's actually going to finish the command and collapse
this properties window and exit out of it all together. So if I press ENTER once,
it leaves the window. But if I were to undo that and go back in here again,
uncheck that and let's change this length to like 1.25 or something, it
doesn't matter. If I hit ENTER once, it confirms
the setting in the dialog box, but if I hit enter again,
then it finishes the command. So this is really just a preference
issue here so it's just whatever you prefer. Our next
area that we're going to look at is, so along this top, you have a little
navigator. So we have our extrusion menu here, and then
we have our sketch. so if we click the sketch,
we'll actually see the sketch itself and this is pretty cool because we can
actually edit the sketch on the fly if we want to. So if we want to change this
dimension we can certainly do that from the extrusion window and then if
we're ready to go back to extrude, we can just click extrusion, and it goes
back into the window. However, we don't want that to be 14, we
actually want this to be 16 inches. So we'll just leave it there,
go back to extrusion. Now, the next area is,
so we have "solid mode active". So to illustrate this, we're going to back away
from the square real quick. So I'll just go
ahead and extrude that, create a new sketch.
I'm just going to drop a circle somewhere in space just to show you this.
Okay, so you have this other option, so in this case, we have a cylindrical
profile, or any other profile that's
able to create a surface on its own. What you could do, is you could go up to the
solid mode and click that, and it changes to a surface geometry
profile instead of a solid body. So that's a quick way to toggle back and
forth between the two if that's what you want to do.
We're going to just toggle it back. And then this is just our preview option,
whether or not you want to see an active preview of what your extrude
looks like, before you actually confirm the action.
So we'll just cancel that. Okay, so we'll actually come back to the
preset section in just a moment because I want to go ahead and cover
the meat of the extrusion function, and that is the input geometry
field. So, what this does, is it allows us to select
the specific geometry we want to use to create this solid body.
So here, you'll notice it says one profile. We'll go ahead and
clear this selection by clicking this little "X"
icon and you'll notice we're left with our profile. So,
if you want to select a particular profile, you want to make sure you're
within the sketch profile selector and you'll know whether or not you're in it
if you have this little blue line at the bottom. So we currently see the little
blue line. If you click it again and it shuts off you'll notice we can't pick up
a profile. If that happens, don't worry just go back to your
selection filter area, click on that, and now when we hover over
our profile of interest it turns green. So we just click in that area.
And, you notice a section called "From",
and so this defines it from our sketch plane because that's where we created
our sketch. This is where it'll define this by default. However, we can
also define other planes if we choose to do so. So if
I have another working plane or something in the area
in the same orientation, I can use that. But in this case, we'll leave it on the
sketch plane. Now, we have our behavior. So this is the
next most important area and this tells the software, "Hey, I want
the solid body to either go in one direction or the other".
Or, we can also tell it to extrude symmetrically
or asymmetrically. So that means that from our plane, we can go
maybe like half an inch in one direction and three inches in the next direction.
And so depending on what you're intending for your design,
that could be a favorable feature. But, in this case,
we actually want to go in the positive Z direction. So, its current orientation is
fine. And you'll notice we could do a couple
different things here. We can go ahead and type in the distance we want to
extrude this to. So, I actually want this to be a one inch
plate, so I can type in a "1" and it'll automatically
show me a preview of that. Also, I can click and
hold this little arrow and I can drag this back and forth. So this is actually
sort of a nice way to manipulate it on the fly and sort of
see what it's going to do beforehand and you know you don't have to type any
numbers or anything like that. Now, you have this little drop down
arrow up here, if we click that, it changes our selector style from icons
to drop downs or vice versa. So currently I'm in icon mode, which I prefer.
But, if you prefer more of a consolidated format
with your drop down box, you can certainly do that too and it shows all
the same options just in a drop down menu.
We'll go back to icons. Now, we have our distance box. You'll notice a
little arrow off to the side. This is pretty neat actually because we can
set this dimension based off of a feature dimension or
by measurement. So maybe I want to measure,
let's say this line here. Well, this line is 16 inches. So it says, "hey,
this extrude distance needs to match that distance in the model so make it 16
inches". It's not so practical in this case, but
you'll find a lot of times where you'll say, "hey, I want it to
be the same length as this other feature". Well this is a quick way to do that.
We'll go ahead and clear that and set it back to "1". And then finally, you
have this "To" option. I'll get more into detail
when we start actually cutting holes in the 3D body. So
we'll put that on hold for now. Okay so, the next section down is "advanced
properties". So, this is a really convenient way to
add a tapered angle in your extrude without
having to create a draft, or a loft, or anything like that.
Now, let's say for example you're designing a part that's going to be
injection molded. Well, depending on the size of the part,
you actually might want to put a little bit of a draft or a little bit of an,
a loft angle on the outer profile of the part that
interfaces with the injection mold because
if your molded part is a little bit too deep, you could have some issues with
sticking to the mold itself. So a way to alleviate that, is creating a
very shallow taper towards the end of the part so
that once the ejector pins start pushing off of the
part, when the, you know, the mold opens up it
helps the part release from the mold itself and you don't get any sort of
sticking or any damage to your molded part. So that would
be a handy use for this particular area. And then, so you know you would add your
angle here. So let's drag this out a little bit more just so you can see
more of an exaggeration on the angle and let's say we wanted to add a one degree
angle to that, or maybe we wanted to let's do something a little bit bigger,
We'll do 15 degrees. Now you'll notice it it
lofts that angle out on this side; we can actually click this flip direction,
and it'll reverse that taper. So that's always there. This iMate button
basically infers iMates to the part. So say for example, you have a pin and
bushing that you want to mate together in an
assembly, you can use this iMate option as you're
extruding these two separate parts, define those iMates themselves, so that
when you import them into an assembly it automatically mates them
accordingly. So that's a really handy tool
for your workflow if you're creating an assembly with a lot of the same
constraints and you don't want to have to do those individually.
And then, so you have your "OK", so that confirms the extrude.
You have "Cancel", pretty self-explanatory. And then this little
plus sign down here is the "apply and create new extrusion". So you saw a little
bit of that previously, but essentially what this does is it
creates the extrude, and then it keeps the extrude option
live so that I don't have to finish the command, do a sketch, come back
in and then click extrude again and do all
this over and over again. It keeps the window and the command open so that I
can just do a bunch of different extrudes back to back.
So we'll go ahead and change this back to "0",
we don't want a taper there. And we want our plate to be one inch thick because
this would just be a standard aluminum plate stock that we order off of
McMaster-Carr or from any other metal supplier that, you know,
we'd be using at this time. And we'll go ahead
and click OK. Now we have the base for our design. So
that's our main use of the extrude. Now,
something else you could do with the extrude tool, and it might be a little
weird based on the CAD software you're coming from, but
there's no individual pocket or cut command by itself. What you
would do, is you would create your profile, select
that profile, and then you go back into extrude
and then you have a cut option which I'll show you in just a moment. So
for our next feature, we need to do our 12 inch by 12 inch
regular hole pattern for our 10-32 fastener. So what we're going to do is
we're going to go into new sketch and I want to create some reference
geometry just so I can keep tabs of, of what I'm doing
with these circles here. So I'm going to just dimension it to 12 inches
by 12 inches. I'm going to set this to construction
geometry, super handy. If you're curious about
construction geometry and other formatting options, make sure you check
out my other video on that. It goes into detail on the differences in there.
So we go to construction. Okay, now our hole size, I've got it written
down here, it needs to be 0.159 inches. So this is for our 75%
thread for aluminum, you know, for our material which is aluminum in this case.
So, I'm just going to pick up this corner
spot here, set my hole size, and these will eventually be threaded, so
this is the pilot hole size for the thread;
just for you folks out there that are wondering
why did I pick this size. If you're unsure of what your thread sizes should
be, make sure you check out, there's tons of free drill charts and
tap charts online so there's plenty of good information
out there with this info in it. So, okay we've got our one hole there but
we need to create a regular hole pattern. So we're just going to go ahead and create
a pattern in here. So we're going to do rectangular we're
going to select our circle, and our two directions.
I have a separate video on pattern tools as well,
sketch pattern tools, so feel free to check that out if you want to learn more
about that. Okay, so we need 13 units in this
direction at one inch, and then we have our second direction
downwards and we'll do the same. Perfect, so now we have our grid of
regularly spaced 10-32 holes, which will allow us plenty of flex-,
flexibility to mount our test specimens to. All right, so now we
have our holes generated there. Now we can go ahead and
finish the sketch, you'll notice everything is fully constrained.
So we go back into extrude. Okay so you might be wondering,
"hey, do I have to go through and click each and every single
profile that I want to create a cut for in this case?",
luckily we don't. What we can actually do here
is we can lasso everything all in one shot, you know, because
you'll notice if we zoom in, it'll pick up each individual hole but it's not
automatically inferring that we want to pick up every single feature.
And you know of course, you don't want to sit here and click through 169
different circles just to create some holes. So
what we can do is we could zoom out a little bit,
and we can just grab everything and you'll notice it picks up all of
169 profiles that I want to grab and it's getting it from our sketch plane
which is on the surface. But now notice something here,
it actually wants to extrude these as pins outwards
and that's not what we want to do, we actually want to create some holes here.
What we can do, is we can drag this in the other direction and we get a preview.
Now, notice the color difference here, we see
green profiles which signifies an extrude so it's adding geometry
to our 3D space. If we go in the other direction,
it creates some red indicators here which means
that we're going to remove material. So that's a very important distinction and
it's something you'll associate, you know, with this as you
go along. So, that's one way of specifying it. Also
what we could do, is I could go down here to the boolean output
operations. And so here, you'll notice it's set as a
"Join". So that means that, "hey, we're going to create new profile, and it's going to
join this new 3D geometry with the existing
solid body". It's not going to be two separate solid
bodies, which you do have the option to do and we'll get to that.
So, next, you have your "Cut" option. Now if we go to cut, it will
automatically know that we want to remove material,
and then you know depending on the dimension in here, it'll
specify the depth. So we actually want to cut all the way through the plate.
Well, how do we do that? Well, there's a few ways you could do that:
you can specify the distance. So I could specify a distance of one inch because I
know how thick, excuse me, the plate is. But,
that's not good enough because what if we come back and we want to
recycle this design or edit this design to use maybe a half inch plate or
actually even worse, maybe a two inch plate but
now I have my distance set to one inch and our intention is to do a
through hole, now it's only going to cut an inch deep.
So what we can do is we can use our "through all" command, so it'll
just punch through any of the 3D geometry that you have
here. But even better than that, you can use the "To"
tool. So if you click "To", it'll open a selection box,
and you know we have our little blue line there so we know it's active,
and we want it to always go all the way to the end
of the plate. So we can click the back face and it
will always go to this section of the plate and I want to show you something
here. So if we hit OK, you'll notice that the
holes are cut all the way through. But hey, let's change our plate thickness
to three inches. Now you'll notice,
it still cuts all the way through, it doesn't matter how
thick or thin the plate is. It just knows, "hey, this user
wants the holes to go all the way to the other end". So this is a really good way
to ensure your design is more robust and more dynamic. I took a couple of steps
back and now we're back into our window right before we created
the cut and I wanted to explain these other two boolean operations that
we see in here, and then of course we have our drop down
with our selector style. So we can do the same sort of drop down
or icon view. But, to illustrate "intersect"
and "new solid", we're going to jump into a new part. Okay, so for our intersect
boolean operation, I went ahead and drew up one cylinder
here of diameter 0.5 inches and I drew another
circle that's spaced evenly off of the center line but it's
overlapping a little bit. So think of maybe like a Venn diagram sort
of a shape going on here. So what I'm going to do, is I'm going to
extrude this but I want it to only take the
intersection between the two. So what I do is I go to extrude, and
you'll notice it's defaulting to cut because it's inferring
that I want to go ahead and create a cut through the part. Also you'll notice if we go back up to
this option menu, you have your "predict boolean operation". So this basically just
infers or predicts what you want to do with your extrude. So in this case, it
says, "hey, you have some 3D geometry here, in this area you don't, I think you want
to remove some stuff there". You can uncheck that if you just want to
make all of the judgment calls there and it doesn't predict it. I leave it on
because it does a pretty good job at speeding up my workflow and it doesn't
really get it wrong very often. So, I'll leave that selected.
So anyways, if we move down here, we have our
"intersect", and if we click that you'll notice it only
shows the intersection between the two circular profiles. So I could hit OK,
and now it just keeps that one shape there. So that would be an example
of the intersect tool. Obviously, you're going to be using it for other things,
this was just to clearly illustrate it for you. The other
option we have here is the "new solid" option. So, if you want to
create two separate 3D bodies within the same model, you could certainly do that.
So we'll just leave that as an extrude and we can actually bring it out to the
same space. Notice here, it says "join" and when
it creates a join, it melds these two as a single element
or as a single solid body. We don't want that, we want them to do-,
to be two separate solid bodies. So what you do is you go to "new solid",
and when you click that it's occupying its own space, it's actually overlapping
with this other one and it leaves that relation there. So if we hit OK,
and I hover over this, you see it's its own separate body.
Now if we go back, and I leave it as join, notice the distinction here. So I just
pull it back out at the same distance, we hit OK. Now when I hover over it, it
treats it all as one singular body. So that's the
distinction between "join" and your "new body" boolean option.
All right, we're back to our shaker table fixture and we are about to
create our cuts for our 10-32 holes. Once again,
I wanted to draw attention to this other distance command which is the "To
Next", which basically takes that command, which in this case is the "cut"
boolean operation, and it takes it up to the next solid
body or at least to the next face within the same solid body. So if I click that,
it's going to default to the same, you know, same type of operation but it's
using this solid as the reference rather than
just the face on the solid, so that's the distinction.
Typically, I use "To" because it gives me the most control
over exactly what I want to do with this boolean operation.
All right, so we've successfully created our
hole pattern for the mounting of our parts that's-,
that we're going to test, but now we need to create the hole pattern to mount
this plate to the actual shaker itself. So what we
need to do here, is we need to create four holes here, and it's a very
specific hole pattern based on the shaker you're using. So in this case, I already
have my hole pattern defined. Don't worry about the specifics there.
Again, I can get into more detail about how to design these types of fixtures in
a later video but for now we're just concentrating on the
extrude tool. So, first we need to draw up four circles in
the area that we need it. Okay, so I have my hole pattern set up
for the interface between the plate and the table,
and it's sized for a 3/8 fastener, and yeah, so we'll go ahead and go
back to our extrude option because we need to create some through holes, but
then we need to create a secondary command and create
more of a shallow cut to accommodate the head of the
socket head fastener. So, first we'll go to extrude, we're going to
select the four profiles, I'll just click and drag over all of this
because it's going to automatically pick all four of those up, and you notice it
doesn't actually pick up the hole features from
before because there's no sketch elements showing or available to create
the cut or the extrude off of, so it's really
convenient. Now, we want to think about what we
want to do, what our intentions are, for this cut. So we want it to go all the way
through the plate, just like these other holes. So we'll go to
our cut boolean option, we'll go to the "To" command, and then have it go to that
face. Click OK. Ok,
so now we have a through hole, but we need to create a space to accommodate
the larger diameter for the head of this socket
head fastener. So what we're going to do, is we're going to create a cut halfway
through the plate that allows the head of the screw to go
below the surface so that we don't create any sort of interferences with
any parts that we may attach to the top of this plate. This is,
this is a huge thing you want to think about. so we're always thinking three
steps ahead, or even more sometimes, to make sure that we don't
have any interferences or any, you know, any problems within our
test equipment. So we'll go ahead and do that now. So I'm
just going to create a sketch on this plane
with the diameter for these holes. So we'll go ahead and I'm going to actually
project the geometry because I want these centered here. Okay, and actually these three were
unnecessary, we'll just use this one here now that I think about it because we'll
just use that revolve circ-, that circular pattern. And then this will
need to be 0.688. So this just is-, has some extra
tolerance built in just in case the hole locations are a little off and
maybe our machine shops not holding super tight tolerances, that's something
else you want to think about. So we'll just click OK there, go to
circular, click that, we're going to revolve it
around the central axis which is a point in
our point of view because the line is going straight at us.
I want four of those, and then there we go, now we're fully constrained. Finish
sketch, extrude. Okay, now this is a great
opportunity to talk a little bit about using work
planes when referencing your behavior or your cut depth, because
in this case, my plate is one inch thick and I need to
cut down deep enough to where I have enough exposed
thread on-, from the fastener on the other side of the plate so it can actually
screw down to the, to the shaker table. Now, we have to think
about this for a second because we don't necessarily just want to do a
blind cut of 0.5 inches just because it works in this case. What if we resize the
plate, but we still want to use the same
fasteners? We need to have the same amount of thread exposed
from these fasteners on the other side of the plate. So what we can do is we can
create a work plane and then reference our cut up to that
work plane. So what I'll do, is I'll cancel that real quick, and we go
to our drop down under work features and we're going to create an offset.
And what we're going to do is, because we need a certain amount of thread showing
from this side, which is at least only half an inch
of plate taking up a half inch of thread and then the rest
of the fastener can stick out. We'll start this as our reference side,
pull it back a little bit and so this is in the negative direction so we want to
make sure we're specifying the negative sign here, and we want it to always
cut down to negative 0.5 inches from this bottom side that mates with the
shaker table. So we go to "-0.5". Okay,
now you see we have our little working plane or a reference plane,
and we can go back to extrude, pick up our four holes again.
Now, we'll switch it to the cut operation but now when we go to "To",
we'll have it always cut down to this reference plane that's always going to
be a half inch off of the side that actually matters, this is really
important. So now we've got that situated, and now
we can just click OK. And now we have our recessed, or our
counterbored holes. So you'll hear the term "counterbore". This is what a
counterbored hole looks like. You also have "countersunk", which is more
of a cone shape recess for those
conical-shaped-head screws, those countersunk screws. So,
those are the, that's the difference there. Okay, so we have our four mounting
locations to mount the plate to the shaker itself,
and then we have our hole pattern to mount the test articles
to the plate. So, we need some spots to put the accelerometer on and this is a
perfect opportunity to illustrate the final feature within the extrude option tool set, and this is the preset
option. So I already drew up the four circles that we're
going to use to cut into the plate. So we'll "finish sketch", go to extrude.
Okay, so going back up to the top here we have "no preset".
Well, what we'll do is we'll select our profiles and
let's say that regardless of how thick the plate is,
we're always going to only thread it down to,
let's say, a quarter of an inch, right. So we need to cut down
to, let's say, 0.375 inches to allow for a little bit of room at the end of the tap.
So we'll do that. So we'll create a cut here,
0.375 inches. Okay, now we want to create a preset out
of this so that when we go to create more cuts,
in maybe this part or other parts, we can reference this
option from a drop down. So maybe I can set this as, let's do, a new preset.
So it's marked as .375 cut with zero degree taper.
And, so we'll just say okay to that, and that's now our preset. If we want to go
back to "no preset", we could certainly do that,
but we'll go back to our 0.375. Now if you go
over to this preset settings, and again to create a new preset out of your
current settings that you had already set you just press the little plus sign
after you set your depth and other options,
and then we go to this little settings menu here, we can save the current preset,
we can rename it. So maybe we want to rename this to
"accelerometer pilot hole". So,
anytime we're creating a fixture in the future and we need to create a pilot
hole to tap for our accelerometer placement, we
always know that it's going to be to the correct depth that we need
and have those correct characteristics for what we're using. So
we'll just, you know, check that off there. You
know also we have some sorting orders. So this is similar to your file explorer in
Windows, you can sort it by various parameters that you see here.
And then you know, you get some new extrude defaults. So maybe
you're doing a bunch of these back-to-back so maybe you want to use
the current preset as your default, well you can certainly do
that. Here, I leave it on "no preset" because it's not something that I use
too often, it's more on a case-by-case basis,
but hey, you might find a use for it. And say, "hey, you know, we no longer use a
certain preset", so maybe I go down in here and I don't want
this half inch cut anymore. I can go to the settings menu and delete
this current preset and now it's out of my drop down, we
cleaned it up a little bit and left space for what we actually use
so we can go back to that, you'll notice it goes back to all of our
parameters that we want. Okay, so now we just click
OK and there you go, now we have all four of our
accelerometer pilot holes using the preset option within the extrusion menu.
So that rounds out all of our extrusion tools. I hope you enjoyed this practical
example of how to use the extrusion tools and I hope that it helps you in
the retention of this knowledge. That concludes this
segment of the Autodesk Inventor Part Creation Module where we took a look at
the available Extrude functions. Don't forget to like this video,
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