Hi and thank You for visiting my blog.

This blog is about my professional work, projects I have been working on, and some funny and interesting things about mechanical engineers. On these pages You can find some of my projects, as I work for army and I am not able to enclose all projects I have been working on.

My most recent designs You can find in posts below.

For more interesting projects You can follow labels, such as:
- aircraft engine blades

- aircraft parts

- wind tunnel models


You can download some of my models, posts with files for download are labeled free model download.

or You can go to INDEX page and search through list of all projects on this blog.

Info about me is on ABOUT ME page, where You can see my professional CV and some info about my skills and professional knowledge.

For all questions about my work, projects, blog or job offers contact me over e-mail or Skype. E-mail form and Skype Add Me link are on CONTACT ME page.

For those who are interested in learning new stuff about Siemens NX program I made NX TUTORIALS page, where I will post some tips and tricks about how to use NX more efficiently.

Best practice in NX

  • Best practice means that this method gives results that are in most cases better than using different methods. But it is just statistics, so if you find out that some other method give you better results in your work case be free to use that method.
  • Design intent is idea behind your design that give answer to questions, what is the purpose of your design (how parts will be used in manufactured product), why did you designed in particular way not some other way, what is the practical benefit of choice of one design method over other in your design considering how your design is fitting inside overall design of particular product, why did you use particular way to dimension something instead other way, etc. (quote from Linked In article “What is this "Design Intent" I keep hearing about?” by Raymond A. ReynoldsTake for example a 1-inch wide strip of metal. The design mandates a hole to be drilled in the center of the part's width. If you model the design by dimension a hole a half-inch from the edge, it is indeed "in the middle of metal strip, but you have ignored the design intent of the hole. If the design changes in the future to a three-inch wide strip, your hole would still be a half-inch away from one side, and no longer in the middle of the part. Had you placed your hole in the mid-plane of the metal strip, no matter what size the width had grown or shrunken to, the hole would have remained in the middle of the strip. The design intent of the hole was maintained, and all it took was a little forethought during the modeling process.”)
  • Knowledge based design or Knowledge-based engineering is the process of capturing of product and process information to build the knowledge of how and why is product created in the product development process. Then it can be reused and enhanced with parameters and rules, integrating design with knowledge (design) in to templates.
  • Poka-yoke concept is way of design that predict accidental human errors in latter stages of design manufacturing/production or use, and prevent them by designing parts in the way that prevent possibilities that these errors can happened. SIM card for mobile phones is good example, poka-yoke concept in this design is one corner cut off on rectangular shape, so there is no possibility that card can be inserted in to phone slot wrong way. There are meny sub-definitions of Poka-yoke concept for various professions, it can be explained as “accidental errors bulletproof design concept”, Its purpose is to eliminate product defects by preventing, correcting, or drawing attention to human errors as they occur.
  • Master Model concept is design concept where model and informations derived from model are in separate files (drawing files, FEA files, machining files, etc.).

  • Name parts so other users can understand what part is from its name.
  • Save parts in designated folder (folder structure should follow design intent). This way parts can be found easy, only by following logic of folder structure of particular project.
  • Make parts in 0,0,0 coordinates (put corner in CSYS zero point for non-mirrored parts, put center of mirrored edge in CSYS zero for mirrored parts, put axis of rotation through CSYS zero point for revolved parts).
  • Front is on NEGATIVE Y side, so put front side of your part there, then views in drawings are following real position of part.
  • If you prefer using NX keyboard shortcuts you can print all of them from Information/Custom Menu Bar/Shortcut keys

  • Sketches should be fully constrained.
  • First use geometric constrains, apply dimensions last, that way sketch will be as robust as possible. Do not use fixed constrains in sketches (if it is not really necessary, and even then try not to).
  • Always choose geometric constraints over dimension constraints for faster updates (less dimension to update faster it is). By using equal radius, equal length and construction lines, you can reduce the number of dimensions placed on a sketch making it simpler and faster and more robust on updates.
  • Use of geometric constrains, and reduced number of dimensions, also help to increase understanding of geometry and design intent of your parts.
  • Do not make fillets and chamfers in sketch if not necessary. Leave them as last features to be done in modeling.
  • Apply constrains during sketch design, do not leave it for last as sometimes it can mess up your sketch details, leading to really long sketch recovery process.
  • Do not reference (link) sketch details to tangent edge of bland or sharp edge of chamfer. These are not features that should be used as references as they are the features that are changed the most on every change of details in your design. Better make intersections with main solid bodies or use previous sketches as references.
  • Use expressions. 
  • If you apply Show as PMI to sketch dimensions, you can edit them by double clicking on them in modeling.
  • Use Feature Parameters in drafting to reuse sketch dimensions as drawing dimensions. In Master model concept, you have to place views from Part, not views from drawing.
  • Show PMI in drawings.

  • If you can use Datum (make datum based on existing geometry) to make references for next feature, instead to use existing geometry. Datum can be detached from faces/features if needed. This way if you remove face/feature datum will still be there and can be reattached to other geometry.
  • Name new views accordingly to what they are used for (name “ISO-TRI #25” does not explain anything)
  • Use PMI do define design intent in parts and assemblies, this is best practice when more engineers are working together on projects.
  • Use layers properly
  • Apply material to designed parts.
  • Use attributes as additional information source. It is easy to see new attributes in assembly navigator.
  • Think about the person who’s going to take over your model. Name your features and expressions. Organize features in a logical and progressive order. If a feature is added late in the design cycle but is best placed early in the part history, use Make Current Feature to roll back the model, add the necessary changes, then Update to End and ensure all features update.
  • Organize your features into logical groups with Feature Groups.
  • Make blends and chamfer last.
  • Make drafts as soon as possible on solid body, and always before fillets and chamfers (do opposite only if you really intent it to be designed that way).
  • When designing parts that should be assembled in particular way or order, but it can be mistaken, use Poka-Yoke concept.
  • On project release: all solids in part should be visible, visibility in assembly should be controlled by reference sets and arrangements. Only solids should be visible, all layers with other (datum, curves, sketches, sheets, etc.) features should be turned invisible. No features should be left as hidden features. This will give better preview icons in history tab or in windows explorer window. (And it make parts cleaned up and more professional looking)
  • If your part is updating properly after editing first sketch, most probably you designed it good. (To check “update-ability” of your designed parts try Edit/Feature/Playback, you have to be in modeling to use this command. It will rebuild your part using part navigator features one by one. That way you can analyze other engineers design step by step)
  • For mirrored parts that have to have separate part numbers in assembly, make right hand side part, then use wave linking to copy geometry (including mirror plane) and use mirror command to make left hand part. This way you have to update only one part for design changes. (But you have to open and update other one, it will not update itself if you do not open it and update both model and drawings)

  • No dimension editing. All dimensions should be live!
  • Do add Ø to half cylindrical view select center-line first then line/point that you want to show Ø for. Then edit dimension and remove arrow on side of center-line.
  • Use Feature Parameters in drafting to reuse sketch dimensions as drawing dimensions. In Master model concept, you have to place views from Part, not views from drawing.

  • Use user named expressions whenever you can. Simple type NAME=VALUE in text field, (do not type name instead default pXX) and this will create expression NAME with VALUE. Named expressions/dimensions in sketches can be edited fast by selecting sketch and editing expressions in Details section of Part navigator, without entering the sketch in edit mode. Naming expressions can help to know what expressions to edit.
  • Named expression are also much easier to use in inter-part expressions linking, when some important informations can be transferred from one part to another via expression linking.
  • Use Extended Text Entry to make complex formula inside your part. Formulas can define dependencies and correlations between parameters (dimensions) or attributes. Formulas works similar like formulas in excel. It is possible to make conditional solutions with IF THEN loops.

  • Use load options, it give you control over what will be visible after you load your assemblies.
  • Open by proximity (in assembly command) is great way to, in big assemblies, open just parts that are close to part you are working on.
  • Use simplification tools.
  • Use assembly navigator to see all attributes needed for proper design of assemblies.
  • Do not use reference set instead arrangements to show different setups of parts in assembly.
  • Make drawing arrangements (for showing details on drawings) by selecting what you want in drawing, so minimal number of components are included in drawing arrangement. This will reduce file size, used memory and make drawing load faster. Name arrangement so it is easy to follow your design intent.
  • Use Assembly/Context Control to control visibility of parts in your assembly while working on it. These are great tools, use them.
  • Use NX bookmarks to save actual assembly context, component groups visible, load option and display settings so you can load your work from one session in to another.
  • To quick check moving parts in assembly, start assembly constrains command and move parts to see if they are constrained to simulate axes of freedom properly (to properly animate moving parts use Sequence).

Rendering views:

  • Have fun
  • Sequence

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