Building a Rope Ladder Sub-Assembly in SOLIDWORKS Using Sequential Part Isolation and Mating Tools

In this lesson we are going to create the sub-assembly that makes up our rope ladder. Make sure that you have your master file open. Let's go ahead and start a new part.

Close out the sketch and insert the master file. Click in the green check mark to make sure that it lands exactly where it needs to stay. Let's go to delete key body in the features tab and we'll start with this double attachment bracket here.

We'll save this as rope underscore 001. There we are. Then save your work.

Do another save as rope underscore 002 and edit the feature deleting that body. Now grab these two bodies to make into one part. Save that.

Do a save as. Make this one 003. Right click, edit feature.

You can right click and delete one at a time or click this double arrow and hit clear selections. Now select this part here. Save your work.

Do a save as rope 004. Now edit the feature deleting that and grabbing these two bodies. Do a save as and do one more rope 005 and we'll make this one just one of these attachment brackets.

We're going to need one on its own. Close it out with a green check mark. All right, let's go ahead and get started with that sub-assembly.

We'll close out all the existing files and open up a new sub-assembly. Start by grabbing rope 001,  locking it into place with a green check mark. Let's save this sub-assembly as SA006 rope ladder.

Excellent. Let's insert the rest of the components. Rope 002.

Let's see where that ended up. I could have made it in place but I'm actually going to delete it and then reload it just to save a little bit of time. There we go.

Save your work. Rope 003. There we go.

I'm saving my work after each upload. Then rope 005. For this one,  let's just place it in the graphics area arbitrarily.

We need this to be free floating. Let's save our work. Next, there's a couple more parts you need to add to this.

The first is going to be our sketch reference part because we need the pattern that's built into that sketch. Beautiful. The second reference is going to be the eyelet that attaches these to our playground.

We know that we have that already in our swing sub-assembly. I'm going to go ahead and open up the swing sub-assembly just to rediscover what that part is named. Let's say 003.

Here it is up here. Swing 004. I'm going to right-click and open the part and then minimize the part.

Let's close out the swing sub-assembly and maximize our new sub-assembly. If we do insert components, because that part is already open,  SOLIDWORKS automatically recognizes it and we can just place it arbitrarily in the graphics area. Let's go ahead and save our work.

Before we start mating these bodies together, we need to make a few adjustments to some of these parts. The first will be this part right here. Let's right-click, open the part,  and mirror it on the other side.

Mirror it against that face, both these bodies. There we go. Save your work.

Then go to combine and combine all four bodies together. Perfect. Yep, there's an update to the assembly.

There we go. The next is going to be in this part here. Let's right-click and open the part.

The first thing is we want to create a plane that exists in the middle of this entire piece. We can just do a mid-plane for that. We'll grab this top surface and this surface here.

We're going to use this as a mating tool. We need to create one more tool. We're going to do that with a sketch.

If we go to 3D sketch and then open up a center line,  let's grab the midpoint of this tiny surface there, connected to the midpoint of its opposite tiny surface. Find the midpoint of that central line and then the midpoint of that tiny surface on the back-end. We now have a vertex that we're going to use.

Let's grab a regular line,  start in that vertex, and just drag it out. Highlight that line. Highlight one of these lines and make them parallel.

Highlight this blue vertex and this bottom surface and select the reference on plane. Perfect. We should have everything we need as far as mating tools in this part.

Let's close out the check. Let's close out the sketch and save our work and close out the part. We can see it's starting to recognize some of the things we placed in there.

Let's go ahead and start that mating process. The first thing we're going to do is go to view,  hide show, and click temporary axes. A temporary axis is an axis that is created automatically just by the nature of the geometry that it describes.

In this case, this is a cylinder and so it automatically has a center line running through it. We just decided to view that center line so we can use it as a mating tool. Let's go to mate, click that center line,  and then click this sketch line that we just created.

Perfect. Now those lines are collinear or coincident in this case. We'll close it out with a green check mark.

The next thing we're going to do is grab this inside edge and this surface of this rope here and create a tangent relationship. Instead, let's close this out. Let's first bring it down so that it lives more or less where it needs to be.

It's giving us a tangent relationship,  but not quite expressed the way we want. Sometimes we have to coach it first. All right, now let's try it.

Inside edge, outside surface of the rope,  tangent relationship, close it out. Okay, perfect. Let's go ahead and save our work.

This can still be moved back and forth. Let's actually go ahead and create a plane in this part as well. We'll open the part, zoom into that top surface, start a sketch on that flat surface here,  convert that edge as the entity that we want to use.

We can highlight it and make it a center line and close the sketch. If we go to features, reference geometry plane, highlight that line,  highlight the surface, it'll create a plane for us that we can use as a mating tool. One of the reasons we have these parts separate and adding features in the separate parts as opposed to the master file is we don't know what types of mating tools we're going to need until we start making the assemblies.

It's always good to work in parts and assemblies simultaneously for that reason. Here we go. Now, if we drop down this menu of that part, that plane is available for us to select as a mating tool.

We'll click mate, make sure that plane is selected, and then we'll select this side plane so they can be parallel to each other. Make sure the reference is parallel and not perpendicular. We'll close it out with a green check mark.

We should be done with temporary axes for now. We'll go to view, hide show, temporary axis. Save your work.

That was a lot. The next thing we're going to do is mirror this component here so that we have to go through the entire mating process that we just did all over again. We did create a plane in this part that we can use.

Let's find that plane. We'll go to mirror components,  and then we'll select this bracket here. There we go.

Simple. Save your work. Next, let's go ahead and mirror some of these items over to the other side.

It's possible that we already have a plane created in our master file that we can bring in,  but for the sake of moving quickly, we're just going to create a brand new plane here. So why don't we zoom into this flat surface here, start a sketch,  grab a center line. Here we go.

We can actually land it on this center line here. It needs to pass exactly through the center of this bracket. Close that out.

Go to reference geometry, plane, highlight that line, then highlight the surface so it can be perpendicular to that surface, and close it out. With that surface still highlighted,  let's do the mirror function that we were just about to complete. We'll go to mirror components.

In this case, click this component here, this one, this one, and this one. Beautiful. Save your work.

Now, let's attach this eyelet where it needs to be. So, always with mating, it always helps to get it kind of close to where it wants to go before you make the mate. Just so SOLIDWORKS has an easy time recognizing where you want to place that piece.

First things first, let's go ahead and select mate, and we'll grab this side edge,  this tiny side edge of our eyelet, and mate it to this tiny side edge here. Here we go. Now, because it's just two lines, we can actually spin this around and lift it up and down.

So, I'm going to go ahead and move it more or less where it wants to be,  again, to make SOLIDWORKS' job a little bit easier. Now, let's mate this tiny top edge to this tiny top edge in our sketch. Looks like it's not recognizing that.

We'll delete that. We'll try this line here. There we go.

Close that out. Now, that's not quite the way we want it to look. So, we're going to close this out,  and I'm going to right-click and go to View Mates,  and let's see here.

What's the problematic mate? Let's move this out of the way. Here we go. Let's just delete this one we just created and close it out.

I see. If we go to the Mates, reverse that mate that we had going on before. This should fix our problem.

All right. Now, as we did before, let's go ahead and drag this out so SOLIDWORKS can recognize this next mate we want to have happen. Okay.

Now, we can see those working out. Close that out. Basic assembly tools.

Mate. Grab this tiny edge. Mate it with this tiny edge here.

Now, this should be fully mated, and it is. That was a lot. So, if you need to review that portion of the video, please feel free.

I'm going to save my work here,  but you can see that we had to correct one of the mates by reversing the direction of it,  which we've done in past videos before. All right. We need to place another islet up in this area as well.

So, the first thing we're going to do is drag a new piece from our Feature Manager, and let's go ahead and set some parallel relationships. We'll select this surface and this surface. Click Mate.

It wants to make them coincident, but let's not go with that. Let's just go with Parallel for right now. Then, while we're making parallel mates,  why don't we mate this back surface and this back surface, again, making them… Well,  actually, in this case, we do want them to be coincident.

So, we'll leave that alone and close out the Mate tool altogether. Let's drag this where it wants to be. Save your work.

All right. Now, let's see if we can get a tangent relationship going. We'll grab this edge, maybe this surface here.

Select Tangent, and there they go. Beautiful. All right.

Save your work. All right. For right now, let's hide these extra sketches.

Now, we need to mirror this piece over to this side, but we don't need to create an entirely new mirror function. You can see that in the assemblies, all the parts are listed first in the Feature Manager, and then after that, we have all of our features that affect those parts and how they appear in our assemblies. That means they're always going to occur after the parts themselves.

So, we can just simply edit the mirror that we previously had. Let's locate the right one. That's the wrong one.

This is the right one. Right-click, Edit Feature, and we're going to add this eyelet to the mirror. Perfect.

Okay. Let's go ahead and close that out. Use the eyeball to re-expose that.

Beautiful. Then, let's go ahead and pattern these eyelets down by one instance. Let's go to Linear Component Pattern, Components to Pattern.

We're going to grab this eyelet and this eyelet. For the direction, we need to pick a vertical line. Here we go.

Let's do Up to Reference because we already have our pattern laid out for us. So, we're going to select this bottom tiny edge,  and then for the selected reference, we want to select the bottom tiny edge of the actual piece itself. You can try the vertex as well.

Let's see. There we go. All right.

Now, for this, we want the instance set to be just two. All right. And it looks like it patterned both sides.

Great. We'll close that out. Save our work.

The last thing we need to do is pattern this entire rope set here. So, we have one more pattern to make. Let's go to Linear Component Pattern.

For the Components to Pattern,  it's going to be this eyelet, this part, this piece, this piece, and this piece. There we go. This piece, this piece, and this piece.

There we are. And then, for the Direction, pick a vertical line. And it's already recognizing the distance that we were using before, which is clever,  but let's go ahead and do Up to Reference yet again because we do want to be able to control that with that sketch.

And in this case, the reference is going to be the very last dot in this pattern. Zoom in. Grab its tiny bottom edge.

For the selected reference,  we're going to zoom in to this eyelet here. Grab its tiny bottom edge or a vertex on that edge. When it shines purple, that's how you know you grabbed it appropriately.

Let's set the instances so that it equates to the number of holes that we have here. It looks like four is the magic number. All right.

We'll close that out. Save your work. Now, let's load this into our General Assembly.

File. Open. Locate your GA001.

And since your sub-assembly is still open, you should be able to have it automatically available as you begin to load it in. And here it is. Rope Ladder Sub-Assembly.

We'll hit the green check mark, locking it into place. All right. Save your work.

And that's it for this video. In the next video,  we're going to create the parts and the sub-assembly required to make our stairs.