Welcome to Top Down Design Tips and
Tricks. There are 6 tips and tricks in this video. I'll put timestamps for each
in the description section in case you want to jump ahead. A slide precedes each
section and the entire slide deck is available for free from the Downloads
section of www.creowindchill.com. 1. Sharing Dimensions in Data Sharing Features. Here I have a Skeleton model for a drone that I'm working on, and I have an
Annotation Feature that contains 4 different Annotation Elements. I'll go
back to my assembly and it contains the Skeleton as well as the target part that
I want to create based off of my Skeleton geometry. I'll start off by
activating the target part and I'll go to create my Copy Geometry feature. Then
I'll select the geometry that I want to use. Now to get the
dimensions or annotations to go along with it, I'll go to the References tab
and click on the Edit button below Annotations. Then I can pick which
annotations that I want to take along with my Data Sharing feature. I'll
complete my Copy Geometry. Now let's go and open up the target part in its own
window, and there you can see my Copy Geometry along with the different
dimensions. Let's create some solid geometry using the Thicken
command. And now we'll make a drawing and we'll
see how the annotations will appear in the drawing as well. File > New > Drawing.
Normally I would change the name but I'm not going to. We'll use our template
and there we see how the dimensions from the Skeleton appear in the target part
because of the way that we copied the annotations along with a Copy Geometry
feature. 2. Using Copy Geometry with Patterns. Let's use a Copy Geometry
feature to reference a pattern from another part. Here in my assembly I have
a component which has an imported feature and I used FMX
to recognize a couple of the patterns. Now I want to
create a part that references the basic shape of the original part and also uses
one of the patterns. I will activate the other part, the target part,
and I'll go to create a Copy Geometry feature. I'll select the surface that
I want to reference and that's all that I'm going to reference here. I'll hit the
check mark, and now let's open up the part in its own window. I don't want
all those holes in my new part so what I'll do is I'll select the surface, copy
it, and then paste. When I perform the paste, from the Options tab I can fill
the holes on this surface. I'll hit the check mark and my new copied surface is
created. Let's hide the original Copy Geometry. Now I'll
select my surface and use the thicken command to create some geometry and hit the checkmark. And so we've got
our part. Let's hop back over to the original assembly. We can see our new
part sitting on top of the existing geometry and what I want to do is I want
to reference one pattern of those holes. The trick is, I'm going to create a
Copy Geometry feature and it's only going to contain one of the instances
from one of the patterns. That's all that's going to be in there. So... Activate.
I'll create another Copy Geometry feature. Let's use the right mouse
button to change from Surface Sets to References. Pick an axis and hit the
check mark. Now let's go back and open up the other part, and I can see my axis.
Let's create a hole and I'll select the axis, hold down the
Control key to select the surface. Let's change this diameter. I'll
right-click over the depth drag handle to change the depth option to To Next.
Hit the check mark. Now what I can do is, I can right click on the Copy
Geometry feature and pattern it, and it creates a reference pattern back to the
original source model. Let's hit the check mark. Now that I've
patterned the Copy Geometry feature, I can pattern the hole. We have our
preview dots and I can say, hey, you know what,
I don't want to generate this one over here. I can click on the preview dot
then I'll hit the check mark. And with that, I've created a pattern in my target
part that references a pattern from the source part. 3. Shrinkwrap with Manual
Collection. Let's use the Manual Collection option to select references
for a Shrinkwrap feature. Here I have an assembly and I want to add some
references to my Skeleton model. I could use the Copy Geometry feature, but Copy
Geometry only allows you to select references
from a single part. You can also use Shrinkwrap, and people typically use
Shrinkwrap to grab all the surfaces from an assembly. Sometimes that can be
too heavy, so I'm going to use the Manual Collection option. First off, I will
activate my target Skeleton. Then I'll click the Shrinkwrap feature.
Instead of the default option Outer Shell, I'll change to Manual Collection.
Now I can start selecting the surfaces that I want to
use as references. I'm just using the Control key to select the ones that I want.
A little Query Select, and some other surfaces, and this is especially
convenient when you are trying to route cables or pipes and don't want to
collect too many references. Also, from the References tab, in addition to
selecting surfaces that you want to use, you can also select Datums. For example,
I can use this to select a few additional datum axes that will help
with my cable routing. Then I hit the check mark and my Shrinkwrap feature is
created. I go into our harness part and you see that it's relatively
lightweight. 4. Smart Tables of Parameters in Notebooks. In this tip, we'll learn how
to create a table that automatically lists all the different dimensions and
parameters in our notebook. First, I'm going to start off by creating a 2x2
table and place it on the drawing. Next, I'm going to configure my column
widths. The first one will be the names of the
parameters so I'll make that about three inches across and then let's
fill in the values that we want to be in the cells. The first column
will list my parameters and the second cell will list the values. We'll go back to
the Table tab and I'm going to create a Repeat Region just from the bottom left
cell to the bottom right cell. Now when I double click in the cell, I'll be able to
put in report symbols. In the left cell, I'm gonna put lay > param > name and then
in the right cell I'm going to put lay > param > value. Then when we Update
Tables, our table lists all the different dimensions and parameters from the
Notebook. 5. The Sheetmetal Offset Command. In this tip, I'll show you how to create
sheetmetal geometry based off of a Skeleton. In my assembly I have a
Skeleton model with some geometry and I have a target part. First thing
I'm going to do is activate the target part and create my Copy
Geometry feature. Let's select these surfaces that we want
to use and change the name of the Copy Geometry feature.
Then hit the check mark to complete it. Now I can open up the part in its own
window and I'll select my reference geometry. Then I'll use
the Sheetmetal Offset command. Note that this is different than the Offset
command in standard part mode. We're going to use an offset of zero but
here's where I can specify my thickness. I'll make it a little larger so you can see
it and let's make sure that it's applied to the inside of the model. What's
nice about this is that if I go to the Options tab, we have the option to add
bends on sharp edges and so I'll make a nice big value there
and hit the check mark. I'll hide my Copy Geometry feature and there
we have geometry based off of our sheet- metal Skeleton. 6. Converting a Standard
Part into a Skeleton. In this tip, we'll see how to turn a standard part into a
Skeleton. I have my assembly and I'm going to start by assembling the part
that I want to be a Skeleton model. I'm just going to locate it
using the Default constraint. To turn this into a Skeleton, the first thing I'm
going to do is I'm going to take it and I'm going to drag it up to be the first
component. Now you might have some trouble getting it to be the very first
one. If so, just drag your other Default Datum Planes below it. Now
I'm going to right click on it and use the Replace
command, and I'm going to replace this By Copy. Here we have the option to copy
it as a Skeleton. Now I'll just click OK and you'll see that it's
symbol next to it in the Model Tree has changed to indicate that it is and
a Skeleton model. Our books are available on Amazon.com. The electronic versions
are free to read with Kindle Unlimited. Thank you very much. I hope you enjoyed
this video.
