CAD Roller Coaster Model Car Concept

Working on a new concept model in part and assembly design. This is the lower chasis. modeled in Catia V5 and screenshot in 3D Via. More to come soon including the 3d xml files.

Best Practices for CATIA V5

There is a great thread for CATIA V5 Users:

http://www.coe.org/Collaboration/DiscussionForum/ActiveDiscussions/tabid/210/forumid/6/postid/129677/view/topic/Default.aspx

I've compiled the complete list of suggests here:

1 Never make a plane from a solid face! Reason being is that if the solid changes, it can affect the plane which can snowball into a huge mess of errors.

2. (for managers) Never purchase Catia, and expect to implement it, and get full functionality, without TRAINING, and I mean professional training.

3. Never make geometry without knowing what the 'In Work' object is.

4. Never open a R18 file in R19, and accidently save it.

5. Never use File + save + Propagate directory, as a substitute for file and directory structure management.

6. Never alter the Customer model

7. Don't do fixed bid work for less than the going contract hourly rate. To do so is just plain self torture.

8. Never do fixed bid NC programming

9. If you ignore #8 .....Never do fixed bid NC programming, for an new customer, without a signed off preplan.

10. Never Mix hybrid and .........

11. Never trust that hotfix/SP will fix the problem you reported on first round without any additional problems...

12. Leave fillets out of sketches and make them as dress-up features operations except, curves that define major features of the design should be included in the sketch.

13. Never release a service pack, to the population, before a major test regiment

14. Never load a service pack, before a major deadline.

15. Never skip going to a COE annual Conference

16. Never do nothing but whine and complain about CATIA. Sure it's fun to poke at it, and have a good laugh at DS's expense. The reality is, as Roger says: ::CATIA keeps getting better all the time"

17. Never duplicate geometry within a sketch. Keep sketches simple, and only define a single profile. Use Pattern to duplicate the profile's feature

18. Never link to anything that isn't published
19. Never use Faces, Edges, or Vertices to create new geometry. You can use the, but always create an EXTRACT element first.

20. Never exit a sketch unless everything is fully constrained. (never exit if geometry is white - everything should be green or yellow)

21. Never exit a sketch without first doing a sketch analysis.

22. Avoid using Red. Catia uses Red to 'warn'. It can become confusing.

23. Don't use translate/rotate/scale in normal design. They are useful if you get data from other CAD, but other changes should happen with changes of part specification, not by adding these commands.

24. Don't try to do everything in one part like V4. Learn Products and do your work in your own CATPart.

25. Don't use the V4 method part modeling; don't make a body and pad of every solid feature and boolean Add or Remove the body to the part. V5 features are automatically added or removed, making boolean operations unnecessary for basic part design. Use boolean operations only for grouping and special situations.

26. Don't turn on the Datum mode when making surfaces, to create isolated surfaces like in V4. Keep the parent/child relationships to make it easy to modify surface models.

27. Don't blindly create all sketches as positioned just because you heard it was better. If you do create positioned sketches, make sure you position them properly. Positioned sketches are extremely useful but aren't required in a lot of situations. (Floating sketches have their own set of issues.)

28. Use "Positioned Sketch"

29. In general: The rule of one Physical Part = one CATIA Part. Body is not Part, it's Body. (Exceptions: e.g.: Over-molded parts.)

30. If you create Contextually linked part (part with contextual links) Position the part to common origin. Typical way of getting an assembly level update cycle is:
• Part is positioned with constraints that create a Positional link between geometry of this part & other parts
• Part has contextual links that affect to this very same geometry
èeasily there is a conflict of geometry position versus geometry shape... èUpdate cycle or impossible to update.
èIf you create contextually linked part, just freeze it to space with Fix or position it with constraints from Basic planes.

31. When creating external references or internal references be thoughtful of how they are affected by changes. Think; "how flexible is this reference?" It's not always easy and sometimes requires trial and error.

32. Profile sketches should be limited to lines and as few curves as necessary to describe the geometry.

33. Learn how to build a well named / organized tree and file system. It might seem trivial on small jobs, but on the big ones it becomes an absolute necessity.

34. When creating assemblies with several constraints, LABEL THEM so you know what you're looking at when one of them breaks or fails. Do it when you create the constraint.

35. Always comment actions/knowledgeware scripts/VB scripts so you know what you did.

36. Learn and understand Links

37. Learn and understand Parameters

38. Learn and understand PowerCopies

39. Learn When and Why to use Boolean Operations. They aren't always required, but they are OK to use when they are required. If you have to go out of your way to avoid them, then use them. KISS - Keep It Simple, S(illy)

40. Try to limit the number of items that you project or intersect into a sketch (use edges). If you do create use edges, make sure to select the item ONLY from the tree. If you select the item by picking the 3D geometry, the use edge will always use a BREP, which can be unstable on future updates.

41. Check and double check your CATSettings. Understand them.

How To: AutoCAD 2008 Tutorial

I found this video to be very helpful. AutoCAD 2008 Tutorial, the Autocad interface, toolbars, pull-down menus, command line, accessing commands.

Pilgrims Plunge CAD Model Recreation

Pilgrims Plunge is the world's tallest water ride and can be found at Holiday World in Santa Claus, Indiana. This is my CAD model recreated in CATIA V5.The original ride is manufactured by Intamin. The layout is pretty accurate despite the fact that I haven't seen any real blueprints.For more thrill ride facts check out Amusement Authority.

Solid Works Material Application and Catalogs

Have you been asking yourself these two questions:

How do you apply material in Solid Works?

How do you create a Solid Works Material Catalog?

Today, I will be sharing the solution with you. Here is how you apply material to a specific part in Solid Works:

1. Open part to add material.
   
2. Right Click – Material <not specified>
   
3. Select – Edit material
   
4. Select – SolidWorks Material dropdown
   
5. Select – Material Library
   
6. Select material that applies.
   
7. Select – Green Check Mark
   

That's how you do it. Pretty simple, huh? But what if you don't have a Material Library or catalog to choose from? You need to create your own. Here's how:

1. Right click- Material / Edit Material
   
2. Select Material Library
   
3. Select a similar material (2024-T3 Aluminum)
   
4. Select – Create/Edit Material
   
5. Fill in Material Name.
   
6. Fill in Physical Properties.
   
7. Select OK. The material will be added to the top of the list.
   

There you have it. Was that explanation sufficient?

Pro/Engineer CAD Tips and Tricks

I know I've gotten away from this lately, but I think it is time to get this blog back on track and provide you with CAD systems help. Here are a few best practices I've learned from using Pro/Engineer Wildfire in my engineering job experience over the years. If you're stuck or having difficulty with a project hopefully one of these pointers will help you out. I know Pro/Engineer can be a bit tricky sometimes, especially when you are going from one CAD software package to another interchangeably like I have.

General Notes

• Make sure to use the "erase not displayed" to keep the memory cleared so that changes to parts are saved properly.
  
• Make sure you are using proper environment files by running batch file from the Environment folder in the Pro Engineer main folder.
  
• Since ProE keeps separate files for all versions of drawings, parts, and assemblies it is best to use the "open file" feature instead of dragging and dropping files into ProE. This ensures that you are always opening up the most recent file.
  
• Create cross sections of parts and assemblies in the part and assembly work benches prior to drawing creation.
  
• Create datum annotations at the part and assembly level prior to drawing creation.
  
• Always keep in mind the final product, which is probably a drawing file, and all other stages will be easier.
  

Part Design

• Unless otherwise specified, use internal sketches by selecting the operation then entering into sketcher mode.
  
• Planes should be placed either at an edge, center of a part, or intersecting a main hole feature.
  
• Create special planes as needed for part placement in assembly or to design special features.
  
• When practical, use symmetry about axis in sketcher mode because this reduces the number of constraints needed to drive the part.
  
• Strong dimensions equate to a fully constrained sketch in CATIA. All dimensions should be white instead of grey.
  
• Best practice is to create separate chamfers/rounds for different sizes instead of using sets.
  
• Best practice is to group holes, rounds, and chamfers together by feature at the end of the part tree.
  
• For sheet metal parts, it is best to use the sheet metal workbench and create the parts using the sheet metal portion of it instead of creating an extrude then recognizing the part.
  
• Sheet metal workbench is default inches, you may need to change units to mm (which I often forget. Seems obvious but is an easy mistake to make).
  

Assembly Design

• ProE assembly is parent/child dependent or history based so it is best to build assemblies in a logical manner.
  
• ProE allows the component assembling into the assembly to be opened in another window. Knowing how and when to use this feature can simplify assembly creation.
  
• You can use existing patterns to place repeated components quicker.
  
• ProE has lighter constraints so may use offsets when needed unlike in CATIA (where the offset constraint is heavy so when you are dealing with a large assembly it can get bogged down pretty quickly if you are using a ton of offset constraints. In CATIA, use coincidences instead).
  
• May need to switch between mate and align to get component in proper position.
  
• Using automatic constraints, it only takes two constraints for circular parts.
  
• May add additional constraints to over ride automatic constraint mode as needed.
  

Drawings

• Best practice is to figure out the total number of sheets required then create all sheets prior to starting any view creation.
  
• Best practice is to figure out sub sheet size for all components prior to creating drawings so that drawing creation is quicker and easier.
  
• Best practice is to place all subsheets for an A0 sheet before adding notes or views.
  
• Best practice is to add the notes prior to the views.
  
• Best practice is to add model and set model versus having model open in the background.
  
• Green text from first sheet is not copied to added sheets so you will have to copy/paste this information to other sheets.
  
• If parts/ assemblies are set up correctly, then using show/erase allows for faster dimensioning of components.
  
• For non-split balloons, use default balloon creation.
  
• For split balloon creation, use palette split balloon.
  
• For weldment symbols, use custom palette then browse to C:programfiles\proeWildfire4.0\symbols\library_syms\weldsymlib\iso_weld
  
• For surface finish, insert surface finish, choose retrieve, generic or unmachined as required.
  

Engineering Textbooks reviews and deals

If you are currently an engineering student please join my Engineering Textbooks fanpage. Find great deals on textbooks as well as reviews. We believe that engineering is the field of the future! Engineers are needed to design and build everything from the latest energy efficiency electric car, to the next generation iPhone, but it all begins with a good education in the fundamentals of engineering and good textbooks are a prerequisite of a good education. If you are an engineer, or engineering student please join this group, and if you have a good engineering book please mention it on the wall. If you have any questions that relate to engineering please leave them on the wall as well and we will try to answer them!