[Raz11]

Hi CNC. I am new to this forum. I need some help on a project i'm currently trying to do and I have no idea where to begin. I am hoping some kind soul out there will show me the way..

I am fairly new to Solidworks but not a complete newbie. The main commands I know is the Extrude, Cut, Shell and other features. The bits I struggle on is the Sweeps, Reference gemometry, mates, and other stuff..

THe project i am working on is trying to make a pushchair/baby stroller in Solidworks.

I have images of what I want to model, have the main measurements i need, i just to make it in Solidworks, Assemble and then test using the Simulation software... But i have no clue where to begin Someone please help!

Images of the stroller push chair i want to model are at the end of the thread post.

A breakdown of what I want to do:

1) I want to make the frame of the stroller + the wheels. With this assembled, I will be able to do an initial Displacement Test and check my Factor of Safety.

2) I want to make the seat and the Sunhood of the stroller. This will be added to the main assembly.

3) I want to make my Stroller have the ability fold, and the seat to be reclined backwards as shown in two of the images.

Stroller's website: http://philandteds.com/products/push/smart

By the way, I don't want to make the model using surfaces etc. THe main tool i need to make the frame and stuff is the Sweep.

I am using Solidworks 2011 version.

Thanks for reading, I appreciate any help that can be offered,

Raz.

[PMF]

Hi Raz11,

Hopefully you are making some progress on your assembly, but I guess that we can start with the tubing. I would focus first on making the individual parts. Create as many as you can right now. Are you familiar with configurations?

From looking at your pictures, on the assembly side I would familiarize myself with the concentric mate first (reading & playing). you mentioned you needed help with mates, so sorry if I am being too simplistic. The concentric mate is going to make circles, round extrusions, share a center point or axis. This will make your tube slide within another tube.

How far have you gotten on your parts?

PMF

[Raz11]

Thanks for the reply PMF.

Thankfully the progress is looking much better now. I have attached a quick render i did of what I have so far. I still require some assistance though.

DO you think you could guide me on how I would make the sunroof/Canopy for the stroller? I have tried lofting planes at an angle, however SW doesnt seem to like it.. Proper annoying me! :P Its like i'm so close yet so far...

The main things that I need to do is the canopy and undercarriage (where the user stores shopping). And yes, my tutor has specified that we have to design it in solidworks, even though he knows its going to be challenging to make using the program. Something like 3ds max would be much easier to do it in but he's currently teaching us that software so we're not very conversant in the program.

However I can say, that over christmas I had a good play around with SW and much more comfortable with the interface, so don't worry im not a basic noob anymore ahah, but I am still looking for any any help! Will be much appreciated.

Thanks.

My progress render:

[PMF]

Hi Raz11,

You are welcome. I will try to help you as much as I can.

I put this together pretty quick, so sorry if I missed anything.

For the tubes supporting the cloth for the canopy, on the front plane, or any other draw a sketch of the shape you want. I used a large radius with a straight line tangent to both sides. Exit the sketch and this will be your path. on a perpendicular plane draw a small circle with the center point coincident with one of the ends of the first sketch. Exit this sketch too. Now use the sweep command to sweep the circle along the large radius path.

You can now create a reference axis with the top and front plane. This will be your axis for a circular pattern. Create 3 or so. Or save this and put it in your assembly for multiple instances around a hub or something.

Are you sure you don't want to use a surface? It is supper easy! Let me know and I will try to reply over the weekend.

[Raz11]

Wow that is awesome PMF!

I have done what you said, however I am stuck on how to actually get the filling of the cloth? I only have the frame of the canopy using the sweep method. I've tried lofting and SW is having none of it. I'll show you what i have so far.

Thanks for the help!

[SirDenisNayland]

Sorry not to derail or anything, but say you were to animate that hood, setting the rods as a metal obviously, and the fabric part as a type of fabric, will solidworks actually help you to analyze how the fabric folds up?

I am assuming another radius was swept inbetween the rods to create the fabric ( because of how even it looks). Would there be another way, such as creating the fabric peieces and then attaching them?

[Raz11]

SirDenisNayland: Thanks for the comment. On this project in particular, we are expected just to test the effieciency of the pushchair frame using Cosmos works, nothing else, so any other components such as the fabric parts, wheels and seat do not need to be analysed for the project.

I would still like to know how PMF created the fabric filling between the thin metal sweep frames?

Is there a way it could work with Lofts?

Appreciate if you could get back to me, thanks.

And trying to answer your question SirDenis, no i don't think solidworks will be able to animate the fabric to fold because you may need 3ds max for that. Even my tutor knows that it will be a challenge to make the fabric parts such as the seats, under carriage and canopy. Though i may be wrong

[SirDenisNayland]

I was always under the impression that 3DSMax was an animation and other media type oriented 3D modelling software, not so much a production engineering type software. I am mainly interested in its analyzation techniques. I would have thought being that it could model air flow, as well as stress points, twisting etc, that it would be able to allow you to verify such things as a piece of cloth.

Hmm. Perhaps a little too in depth for this thread.

[PMF]

HI Raz11,

Sorry I wasn't able to reply over the weekend.

I created the hood with a surface. You mentioned that you wanted to use solids, bit it would be much easier to use a surface in this case. So I will show you how to do it, and if you want to use a solid, we will find another way.

I gotta hurry because I have a meeting in a few.

Create a reference plane at 30 degrees or so.

Draw a sketch like the one in the picture (or whatever you want).

Draw the same sketch on the reference plane.

Draw a third sketch (on the right plane) connecting the two larger sketches on the front plane and the reference plane. Use a pierce mate on each end.

Now just go up to: Insert -> Surface -> Loft

Under "Profiles" select the first sketch on the front plane and then the second sketch on the reference plane. Under profiles it should now read Sketch1
Sketch2

Under "Guide Curves" select the small arc that is drawn on the right plane.

This should show you your hood. Click the green check mark.

Now, create a sketch on the top plane: Draw a small circle that is coincident with the end of the arc on the front plane. Exit the sketch.

Now create a sweep. The profile will be the circle you just drew. The patch will be the same sketch that is used for the hood surface. Hopefully you have seen before how you can use the same geometry for creating multiple items.

Just in case: When you go to select the profile under "Sweep", just next to it you should see the feature tree. Or at least a "+" sign to open it. Go to under the "Surface-Loft1" feature and select sketch1. That will be your path.

Repeat for the second rod that supports the hood. You can play with an array to create the rods, but you probably need to create additional sketches to create the hood portion.

Hopefully this makes sense...If not I will do my best to make a video for you.

Have fun and will check in later.