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Files that go with this tutorial can be downloaded here: http://home.hetnet.nl/~waikitchung/mousetut.zip
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Many IDers are not familiar with the surfacing in Solidworks. It might be handy to go through a simple product like a mouse to walk through how you might go about modelling in solidworks. Over the next few days I will go over how to go about doing this in Solidworks.
I sketched this concept over lunch so the design might change over the next few days hehee Hopefully we will have a helpful series


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This should indeed be interesting, I do all my modelling in rhino, so I'm curious to see if Solidworks can keep up a bit.

Hello parel,

Well, great initiative !

Keep on providing us with nice stuff....!

Best regards

parel, thanks a lot again. i finally can start learning solidworks!

Dear waikit,

Well, SolidWorks is very easy to use if you ever had any experience with other parametric modellers. If not, I still believe that is easy to use once you understand what the "Parent/Child" topic is, and once you learn to model with the planes and axis! So, don't worry . . .put some energy to it....and for sure you gonna love it!

Greetings

dot kite, thanks for your support. just need more motivation to start with solidworks. this coming tutorial of parel will certainly motivate me, because it will be first posted on this forum right parel?

Nice tutorial, keep em coming...!

For me, solidworks is very intuitive especially if you know other modelling software. (I use Alias and Rhino mostly, since that's what they had at my school.) You can do a BOM and exploded views with a couple of mouse clicks in solidworks. But it's also rather expensive, especially if you are a student.

Also, check their website- they team up with local training companies in many areas to offer a free intro class. All you have to do is sign up. I got a limited trial version cd of the previous rev to take home (unfortunately, it wouldn't install though).

Today I will go through initial set-up for ID in Solidworks 2005. (We can figure out some work arounds for earlier versions as we go along for those with earlier versions) When you use SolidWorks it initially feels as if you are drawing with crayons or something. You free-form draw a thick blue-lined circle wherever you want it with no constraints (very unsettling for those used to pure parametrically driven models). What a novice program! It even looks like crayon. However, the simplicity isn't indicative of an underpowered program, but of intuitive interface. If you want an unconstrained circle somewhere, SW won't argue with you, but go with the flow.

You can soon learn a whole palette of tools that allow very complex geometry in very few steps. However, Solidworks out of the box does not show all the tools that I use on a consistent basis. I will show you how to customize the layout for ID purposes.

This is what I see when I initially open Solidworks. There is not a whole lot to look at. This is because the interface subtly changes depending on the type of edited document



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Type Ctrl+N to create a new document. Click on Part. The opening screen will not look like the one below. I have removed all the commands and toolbars, so that I can start out fresh, and only show common commands. To remove a toolbar click on the edge of the tool bar and drag it out into the display area. This makes the toolbar a standalone dock-able window that you can close out.


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Click Tools -> Customize. A dialog box opens up that looks like this. Click the following options within the toolbar options. This opens up the toolbars with commonly used commands


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Your screen should then look like this (hmm I cant seem to upload the image..will try later)

Next drag and drop the new toolbars into the grey areas surrounding the display area to clean up the display. Arrange the toolbars as you deem logical. Your screen should look something like this:


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We still don?셳 have all the commands that we need. Click Tools--> Customize. A dialog box opens up that looks like this. Go to the Commands tab, and in the scrolling Category menu go to Sketch. Add the commands that I have circled in the menu to the sketch toolbar on the right of the screen by dragging and dropping


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Scroll down to Features Category and drag and drop the extra commands. I will explain what most of these tools do later in the tutorial.


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You can also optionally remove commands that you rarely use by dragging and dropping them into the display window. This does not work during regular use, only during customization


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You should end up with a screen that looks like this (minus the doodles) Tomorrow I will go over the modeling strategy that we will use. It is very important to think about how you are going to model an object and your overall strategy before you actually start using Solidworks

We went over some house-keeping today. This might be tedious, but dont worry things will get a little more exciting the next few days.




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Hey Parel,

Thanks ever so much for this tutorial, I have not been able to find many surfacing tutorials for solidworks. this one looks great! keep them coming!

Here are some approaches that we can possibly take. Approach 1 has the disadvantage of having a degenerate point where all the isoparms come together. This can make the surface quality difficult to control. We will probably have a hybrid of Approach 2 & 3 taken to another level


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This is not the mouse we are planning to model just a quick stand in to show some basic modeling techniques


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Over the next few days, I will try and break down how to make this mouse. It is composed of surfaces that are later knit, shelled and split into various components. This kind of method is what is referred to as a "top down" assembly. The actual construction method turned out to be a variant of Approach 2. My sketch shows a crease in the mouse. I decided not to model it because first it would have taken a little longer to think through and explain and second-it wasnt looking all that good .


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Here is a saddle I modelled in Solidworks using the same method as your approach No1. I think it is a very fast route to creating complex surfaces but I sometimes struggle with maintaining tangency. Approach No2 takes longer but is more reliable I think.


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These are the underlying surfaces to model


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The following part deals with inserting backgound bitmaps to use as underlays. Also the curve formed at the interface of the red part and the grey plastic is important. So we will define the character line by means of a 3D curve (3D sketch).

Solidworks uses flat planes called construction planes to create flat curves (2D sketch). These curves are then used to create geometry. The default construction planes are the Right, Front and Top plane. Designers used to Rhino and Alias can be confused by the construction planes. The default constuction planes are not actually views. Refer to Solidworks documentation to learn more to pan, zoom and dolly the camera.

<span style='font-size:14pt;line-height:100%'>Inserting Background Sketches:</span>
1) Click Right plane.
2) Insert >Sketch, to start a sketch on the Right plane
3) Within the sketch Tools>sketchTools>SketchPictureto insert a background sketch. Insert a cropped view of the mouse in the right hand view. I used Photosop to crop out the different views. It is useful to crop each view as close to the bounding envelope as possible.
4) Draw a line that passes through the origin, and dimension the line to 120 mm. This line will be used as a reference to scale the background bitmap
5) Double click the bitmap. Drag handles will appear that will allow you to scale the jpeg to the 120 mm construction line. position the highest point of the sketch over the sketch origin by dragging and dropping


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Repeat the previous procedure on the Front and Top Plane. It is convenient to position the jpegs so that the baseline passes through the origin.


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Sometime it is more useful to have more than one view of the model


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Creating the 3D sketch:

In addition to 2D sketches, SWX allows you to create 3D sketches. which are splines with control points that can move in three axes. They are very useful to define character lines/ bone lines of a product.

1)insert>3DSketch
2)in the right view use the spline tool to trace over the bitmap. It defualts to create a flat curve in the Right Plane.


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Similar to Rhino and Alias you can move the control points in the Top View to match the bitmap. (Hint: Hit Spacebar to get default views like left , right , top etc:)


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Solidworks Rant Time:
The spline functionality is still not fully implemented. The spline control handles of 3D sketches are VERY buggy unless you constrain them horizontal, vertical or tangent to a construction line.

eventhough you cannot use spline handles to the same degree in 3D that you can in a 2D sketch they are stiil a big leap over 3d splines in 2004. The curves will just be a little heavier because you use control points to define curvature rather than the spline handles

Edit: Do NOT pull spline handles in 2005 3D sketch. They are uncontrollable unless they are constrained horizontal, vertical or tangent to an existing 2D or fixed 3D line (even then you have to use the property box to input length) This has been corrected in 2006 though so...phew!


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Tweak the curve to match your sketch lines. You have just defined a 3D character line!


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This is what you should see when you open the file from the beginning of the tutorial. You will see a trimmed surface loft and a bunch of curves. I wanted to start with just curves, but the side section curves are created with curves that are tangent to the trimmed loft surface. The side section curves are also constrained to pierce the 3D character line that we previously created


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Start a Loft between the Edge of the Trimmed Surface and the 2D sketch "Plan View" All required sketches should be in the folder "Sketches for the Main Surfaces" which is nested in the history tree.


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Start editing the loft so that it is curvature continuous at the top. This is done by editing the Start Constraint to "Curvature Continuous" in the drop down menu.

Define the loft a little more with guide curves. This can get a little squirrelly along the center line because the guide curves at the rear and front (Rear Section of Side Profile and Front Part of Side Profile ) along the center-line are cut (convert entities) from the Profile Sketch. Use the secondary history tree in the modeling window to pick the right sketch

To create a smooth connection along the center line click the guide curves and choose Normal to Profile to make the loft smooth along the center line.


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Mirror the surface bodies along the Right Plane. Generally mirroring the bodies (as opposed to Faces or features) is the most straight forward because the computer does not have to calculate too much information


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If at any point the sketches become annoying or too busy CLick View>Sketches to toggle visibility of Sketches. You can do the same thing with planes, curves, origins etc:

I have toggled sketch visibilty so that I can choose the edges of the surfaces to define a planar surface


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Use the bottom edges of the lofts to define the bottom planar surface


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Knit all the surfaces together to create a Solid. Check the box that says "Try to form a Solid" (the process is similar to creating a closed polysurface in Rhino)
This will give the model mass properties and gives you the ability to use solid modelling tools on the model


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Shell the solid to give wall thickness of 2mm. If you click on any faces that will create an opening in the shell because those selected faces will not be included in the final shell. So in this case Dont click on any faces because we are interested in keeping all the surfaces


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Fillet the bottom edge 2mm


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Created an extruded surface with the 2D sketch that defines the material break between the two colored plastics.

This will be used to split the solid body into two bodies along the character line that we defined earlier


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Split the body using the extruded surfaces.

Pick the surface
Cut the part
Pick the Bodies that you want to keep from the resulting bodies


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Go to the Solid Bodies folder and pick the top part of the mouse and hide it


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You can see the wall thickness now that you can see inside. Fillet the top edge. Fillets are cool from an engineering perspective they eliminate stress risers at sharp edges, and allow for easier ejection from tooling. Fillets also make your final renders look good because they catch light well.


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Hide the bottom and fillet the edge of the top component


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Create an extruded surface to split the top component again.


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Split the model with the extrude. In hindsight it would have been better to combine all the splits in to one command


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You can change the color properties of any object by right clicking on it and going to color


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Cut extrude the opening for the mouse wheel. Offset the sketch plane from the sketch plane by about 5mm (this option can be found in the first drop down menu).


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Extrude the mouse wheel and in the Direction1 and Direction 2 options set them to offset from surface. Create the extrude .5 mm offset from the inner walls of the opening. Uncheck the box that says merge result. SWX by default tries to chunk features together into one solid mass whenever Solid features are used. Most times this is preferred but sometimes you might might to makuse of multi- body features (as in the case of the scroll wheel.

This fillet is a full round fillet. Pick the three consecutive faces of the cylinder to create the fillet

We really appreciate your great effort on this very interesting tutorial. Well done. Thank you again!

oh my... that's pretty.. that rubber looks really convincing!! photoworks, is that part of SWX?

Thanx for the encouragement Renszu. Photoworks is the rendering add-in for Solidworks. It comes with Solidworks Professional. Photoworks is not the best rendering system in the world, but it can be coaxed to produce very nice renders

great initiative ! very impression

I figured it out. Select the Extruded Surface as the trim tool geometry. After doing the split command, I had to hide the Extruded Surface from the tree manager in order for it not to show in the graphics area. It's a very nice ID-based surfacing tutorial for SW. Thanks, Parel.

The fillet2 surface is because I filleted the sharp edge on the Extruded surface. This saves you from creating two fillets later.

Parel, your tip and tutorials are so helpful and greatly appreciated in this forum.

I figured out how I wanted the ribs to look like in the sketch in the folder "Rib sketches" Extrude a surface that goes past the outer surface of overmold

This creates a rib that you can lay onto the surface of the overmold

Create a 3D sketch and create intersection curves between the surface extrude and the outer surface of the overmold.

(Hit Esc after you create the curves to back out of the intersection command)

The curves in green are the curves on the surface of the overmold that you want to map your gripping ribs to. as you can see there are four ribs to be mapped by means of the deform tool.

So we will have to make copies of the revolve.

Use the Copy/move Body Feature to make 3 copies of the revolve. Do not specify a displacement (all the copies will overlap and look like one revolve even though there are 4 bodies). This is so that we can use the centerline of the Revolve sketch as an initial curve
(Ignore the surface extrude . You can hide it)

The Deform tool uses curves to map your geometry to curves. The initial curves map to your geometry, and then Solidworks interpolates the change in geometry from the change between the Initial and Target Curves.

Pick the revolved bodies one at a time to deform them to lay on the overmold area of the mouse.

When you are performing the deform command, hide all the revolved bodies except for one. This makes it easy to select the body you want to work on.

As you can see in the tree, there are 4 deforms performed t omodel each rib

Mirror the grippy bodies to the other side

Combine all the grey parts into one Solid body

Great! I can't wait to try it this week. Incredible gloss or shine in the render! You had previously mentioned in your post a DOF Photoshop in Photoworks. Is this a plug-in?

Hm.. a shot in the dark here, but I can imagine you could render a zbuffer frame in photoworks which indicates distance from the camera in a black/white gradient. You could use this image in photoshop to create a blur in your render with intensities taken from that zbuffer frame..
This is something you can do with 3dsmax, but it's a common feature amongst 3d software so I think photoworks could do something similar.

great tutorial.. each n every step is explained better and meticulously than any other 3d tut. good for reference. thanx a lot to parel.

I think u could try more lights in order to clarify the details, which are the asset of design. 3d max has surely got better rendering engine than photoworks, though i m not sure 'bout the new version of solidworks. but 3Dmax has wide options to play around with materials, environments and camera focusing. the skylight with a white matt ground gives photorealistic appearence.

nice job :-)

Max has a better interface with Mental Ray, which is also the rendering engine for Solidworks office. When I said I add DOF in photoshop . I was talking about Depth of field, and blurs. I approximate what that looks like by using feathered selections, and the FIlter>Gaussian Blur.

Renszu-Photoworks does have the capability of z-depth rendering. Here is a progression to give you an idea of what Rensu was talking about Norah. You can even uses the raw render below and the depth cue rendered image to approximate DOF. As you can see you dont really have to go to the effort of doing a depth cue render if you already have a picture in your minds eye of what is farthest and nearest to the viewer

LIke Ive said before-Photoworks is not the best rendering system by any means but it can do decent stuff

thx you , it's very very cool stuff , thx a lot

If anyone has has feedback please PM me. I would appreciate the info. Pretty exciting that there have been more then 10,000 views!

Hi

I'm a newbie to solidworks, i started trying the 3d splines but stopped because it was so annoying to use.

I managed to find a better method that allows for more control with the curves.
You draw the top and right splines as separate 2D sketches, then select 'project curve' and select both sketches the outcome is the 3D curve your after.

I'm now going to follow the rest of your tutorial, as its extremely helpful.

thanks


EDIT: i've just realised that whats created is a curve not a sketch, and I can't seam to be able to mirror it...
EDIT2: how did you mirror your 3D sketches?

For some reason you cant mirror curves or 3D curves yet. What I typically end up doing is modeling the half model and then mirroring it. Then I tweak the driving curves to update the mirrored geometry. It would be much less resource intensive if you could mirror/virtual mirror a spline cage.

LOL the 3d sketch curve is finnicky. Your method is a standard practise in Solidworks for curve generation. I am hoping that the beta coming out will solve these issues with the 3D sketches. At the Solidworksworld Conference this year a stated goal this upcoming release was to "win the hearts of consumer product designers (ie ID)" Lets hope that this promise carries through.

Great tutorial, thanx a whole lot.

Yes!! great tutor.

I didn't know you can do this stuff in solidworks. I know Rhino3d and I am learning Solidworks and I like the approach of this tutorial in Solidworks,

I have a question. I am having a problem with making a planar surface.

does planar surface work only with 2d Sketch curve?

is it possible to convert 3d Sketch curve to 2d Sketch curve?

thanks, great tutorial.

are there going to be other tutorials?

The program does not make a planar surface when the input curves are not planar. Make sure that all the edges used to create the surface are planar.

To remedy the situation, you could do a surface extrude very close to the planar edge and mutually trim the sorrounding surfaces and the extrude.

Re: 3D to 2D sketch.
Create a plane using three points that pass through the 3D sketch.
Then convert entities to create the 2D sketch.

Re: does planar surface work only with 2d Sketch curve?
Planar surfaces will work with any planar input from surface edges, 2D sketches or 3D sketches. The only condition is that the inputs all need to lie on the same plane.

Hi master,

I am so appreciated for the skill that you taught us. Thank you very much for your hard work, here is my homework according your curve file.
I think it is important to make it clear the function how to bulit the shape before you beigin. and I think it is not easy for me to make the stech that you inform us. i need more lesson to practice.
another question is I find the final render you made is very amazing, but I don't know how to get such effect in photoworks. hopefully we can leern such skill from you later.

af all, I appreciat for your good lesson. I am a chinese and a biginner on the software and the ID field. Thanks again.

allen


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Allen-very nice! I am glad that you made it through the tutorial! You are the first to post work. Could you PM me regarding what you found easy and challenging? This will help me formulate better tut later on.
If anyone has completed the model please feel free to post screen grabs

http://www.productdesignforums.com/index.php?showtopic=781 for render setup
http://www.productdesignforums.com/index.php?showtopic=1177 for more on h

I've been using SolidWorks for about 5 years, mainly machine design and sheetmetal work. I haven't had the opportunity to work with surfaces -- much.

Your tutorial is one of the best on the net, really appreciated. The deform command is something I would have never used and or figured out that you can use it the way you did!

I have thought about attending my VAR's advanced course, but the cost is somewhat prohibitive and not sure it would cover surfacing in depth. Finding useful stuff like this on the net is real help. If you ever run short of work you should write a tutorial / book / guide / CD on surfacing / industrial design with SolidWorks. Such guides are extremely lacking , I and a lot of others would be more than happy to pay for such a guide.

Regards

AcidRatz

thought it's simple and user friendly interface, solidworks is more for mech. engeniers.
I have an experience with unigraphics and solid edge.. (the last one is prety like solidworks)
for speed, accurate surfaces, and flexible work,i use rhino, i will never change it.
with nPOWER plug in, one can perform mechanical tasks as well.

super tutorial !

here's mine. New to rendering, And just so so with Surfacing. Used Photoworks. Still have a lot to learn. Thanks for the tutorial. Any future surfacing tutorials that are more advances and using other surfacing functions?

Parel
Great tutorial !!
I'm a Pro/e veteran of 11 years, but we are looking at Solidworks as a possible replacement in the future. So it was great to see how solidworks handle some real life top down design.
My question is having created this mouse "master" model with it's 4 solids, how does solidworks deal with taking a "linked" copy of one of the solids into a new part for further detailing.
In pro/e you can use a variety of commands to take parametric copies of surfaces etc into new parts, so that you can change a dimension etc in the master which will ripple through to the part file.
Thanks in advance
Stephen

Hi Sayre

This is no problem in Solidworks. You have the ability to both inserting surfaces and parts both linked and non linked into new "parts". (An example) right klik on a surface or a body in the designtree, then insert it to a new part. This can be done with both solids and surfaces.
A nother way to do it, is to open a assembly, and from there klick insert - component - chouse part, or assembly. This is a good way to modify parts, if you have a ground shape of a thing witch shape is the same in all 100 parts, but there need to be a small change on to each of them. If then any changes is to happen to the ground shape, just change it to the master part, and it will change it on all 100. If you get my point!.
Also yo can modify parts on an assembly by edditing the part, and use other combined parts surfaces to ajust this one part. This can be done with or without references. This is also just some of the ways to do it in Solidworks. I hope it helped with some of your questions.

Hi all, I just thought I'd mention CONFIGURATIONS. This is a definite strength in Solidworks, as you can have multiple Configurations within one file - for those parts that can have multiple versions.

For example, all my standard fasteners and parts are done with Configs. When you want to replace an M3 screw with an M4 in an assembly - no need to re-attach assembly relationships (mates) - just replace the configuration and everything stays intact.

You have to see it to beleive it, but configurations are very useful. I know, since I am a SolidEdge convert...

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Hi All,


I've been a reader of these pages for a while now and decided to register in order to upload my Mouse rendering as a means to thank Parel for an excellent tutorial.

I've been using SW for 4 years or so (2.5 years commercially) and still learnt a tonne from the tutorial.

Without further a do, here's my rendering. Modelled in SW2005 and rendered in Photoworks 2. It's not a perfect rendering by any stretch of the imagination but the best I've done to date. It took the best part of a morning to get to this stage, but this included tweaking of the scene through to custom materials, lights etc etc.

Thanks Parel!

Charly


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Charly,

Good work on the modeling and the render. I've just spotted this tutorial and will surely be working through it as it covers the surfacing I want to brush up on in Solidworks. Just like Sayre, I've come to Solidworks after many years with Pro-e and I'm looking for ways to link surfaces like Pro-e might do with the master model merge technique or the advanced assembly extension's copy geometry command. Schwinndk's tip about taking a surface body, right clicking, and choosing "insert into a new part" has helped me out today.

Thanks.

Hi, just completed; well almost, the mouse, but ran into trouble on the deform. Each time I tried it the bottom body shifted to the left (front of mouse) turned yellow as though it was the whole preview, but no ribs. I did notice that after selecting the revolve and target curves that the target curve did not reflect the revolve shape, but stayed a straight line. I tried the deform command on another surface I generated, but the same result - what is going wrong? sw 2005.

Hello,

The tutorial file was already filled with all the sketches but there are 3 of them which I don?셳 know how to make myself. It is the curves that are present in the 3 planes and are used as guide curves for generating the side surface of the mouse. A section of that curve is on the front plane and also on the lofted top surface. How did you make this?

Thank you,
Antonio

PS. Your tutorial was extremely helpful

Hello Bruno
Your problem is that in the deform region your are probably selecting the body of the mouse. This is wrong. You should select the small revolved body that was created next to the mouse because that is the body that you want to deform and not the mouse.
succes,
Antonio