Monday, May 15, 2017

CAD Product Design and Innovation

Design Thinking:




















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How do you do research on patents?

Google has a tool called Google patents, that would be the simplest place to start. Even if you find similar ideas to yours don't get discouraged, that is 99% of the times. The thing is that you don't patent ideas, you patent methods. For example a client who had an idea to turn a high heel to a flip-flop and vise versa per the usage. There were like 50 similar patents, the thing is that none of the one had the same mechanism as client's idea. GloberDesign can also help you how to differentiate your mechanism from others.
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Shaping the part (Evolution of the part design process): 


The Shaping Process, in its broadest sense, involves the forming of the part. Although the initial model is rough and undefined, the evolution of the process results in an accurate representation of the part with precise defining features and limits.

The process begins after you establish the design criteria, gather the reference data, and set up the part file to manage the data. The process ends with a completed solid body that mathematically defines the part's characteristics and product features.

To begin the Shaping Process, you start with a solid. We refer to this as the 'chunky solid' The term is analogous to the initial mound of clay a sculptor uses. It is a solid body that represents the rough shape of your part. Although it is oversized, it is typically more refined than a mere solid cube encompassing your part's limits. Your chunky solid does not need to be as crude as the sculptor's mound of clay.

The rough shape envelope can be derived by creating features or performing Boolean operations that result in a solid body. Considering the adjacent structure, typical sections, reference data, as well as having a vision of the finished part, determine the chunky solid's limits.
The next step in the Shaping Process further refines the chunky solid. You accomplish this by modeling features, splitting the model using surfaces and/or planes, and lastly by creating bodies that you add to or remove from the chunky solid to define a part's shape.

After you model the part's shape, you can add fillets to the solid and apply the final shell. After applying the final shell, add any remaining holes, cut-outs, or trims. 

Following this basic approach takes you from a rough shape to a fully defined part model.

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Creating the Rough Envelope:
The rough shape envelope is the chunky solid that describes the predominant shape of the part. Try to define as much of the part as possible with the first one or two features. This reduces the number of operations needed to define the rough shape.
When creating a part's rough shape envelope, use any combination of features including: extrusions, revolves, free form swept, Booleans, or a primitive to model the solid.

When creating a part, you start by creating a rough shape. This shape encompasses the overall primary form of the part capturing basic shape representing the base solid.

The initial profile is derived from existing geometry around the part. The lines of the sketch are offset from other parts that surround this part. This is the "envelope" in which you need to design your part. 

Splitting the Envelope:
Splitting the model using surfaces and/or planes help further refine your rough shape envelope. Use the command Split from the Part Design workbench.
In real design, you would have had to define the profile after taking into account the surrounding geometry and a general feel about the finished product. The split planes would have been determined by the surrounding geometry. This rough envelope gives you the starting solid to shape a part.

Boolean Operations:
You can create bodies that you can add to or remove from the rough envelope. In some designs, you cannot use surfaces due to special cases in the geometry. In these cases, you need to use the remove function.

Dress Up Features:
Some of the common feature operations used to shape your sheet metal part is fillet and shell. You will want to add the fillets first and then the shell.
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Typically a designer will start with a model containing the necessary curves and surfaces that define the Class A elements and work from them to develop the final prototype/production result. 



Open the start model, develop the surfaces and wireframe using a number of surfacing tools. Every element is built from the Class A features contained in the Geometric Set. These are "dead" inputs that can easily be replaced as necessary as the design changes.



Notice the model only has a single Geometric Set named "Class A Features".
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Datum Features:
Reference features or datum features are objects that are commonly used in the construction of a model. There are three types of reference features: datum planes, datum axes, and datum coordinate systems.

datum plane is a feature that represents an infinite plane in space. Datum planes are commonly used as a placement face for features or sketches. They are also useful for positioning features, constraining sketches, or trimming a solid body.

datum axis is a feature that represents a vector in space. Datum axes are commonly used to define the reference direction of a feature. They are also useful for constraining sketches or defining a rotational axis.


Datum Coordinate System:
A datum coordinate system is comprised of a coordinate system, a point, three datum planes, and three datum axes. You can select each of the components for most operations as normal datum planes and axes. This is an advantage over datum planes and axes since it is a single feature rather than six.



Fixed Reference Features (Non-Associative):
You can create reference features that are fixed in space. Fixed datum do not move when your model changes. A set of fixed datum planes or a fixed coordinate system with components is ideal for starting a model. You can use these fixed datum to create a sketch that may represent the initial profile of a model. Once the initial profile is created you should create relative datum from your initial profile, when practical. These relative datum can then be referenced throughout the model by other features in order to create a well-built, parametric model.
You can create reference features that are fixed in space. You do this by referencing the WCS for datum planes and axes or referencing the Absolute Coordinate System for datum coordinate systems. These fixed datum are not associative to the WCS or any other points you define in creating them. They are intended to remain fixed, though they can be re-positioned using Edit | Transform.

A set of fixed datum planes, or a fixed coordinate system with components, is ideal for starting a model. You can use these fixed datum to create a sketch that may represent the profile of a model. These datum can then be referenced throughout the model by other features in order to create a well-built, parametric model.




Relative Reference Features (Associative):
Picking existing model geometry such as edges or faces can also create reference features. In doing so, you create constraints that define the datum feature. This makes the datum feature associative to the object you pick in creating it. These constraints make reference features powerful since you can define design intent with them. Thus, changing the model also changes the reference feature and any downstream features associated to it.




Layer Management:
Even a moderately complex solid model can contain quite a few reference features. Because you do not need to use all of them for every feature, you will not need to display them all the time. It is best to develop a methodology for organizing these objects.
In the early development of your model, create base datum objects on which to reference later features. A good example might be to create a center plane in a plane of symmetry of the model. Consider placing these datum objects on their own layer and giving them a unique color. Use these datums whenever possible for locating and placing future features to minimize the depth of parent-child relationships.
When creating new datum planes that are specific to a feature, consider grouping them on a specific layer and using a descriptive category name to identify this layer.





In the example shown, a "T"-shape is sketched for creating a subtracted extrusion at an angle to a face. In setting up that sketch, we had to create two datum planes and a datum axis specific to that feature. In this case, a good practice is to place the sketch, the datum planes, and the axis on one layer and give the layer the category name t_slot. Now, all the construction geometry for that feature is located on one layer and we can make it invisible when we do not need it.

Tips:
  • Datum planes and datum axes are infinite in size, the display that you see in the Graphics window serves only as a reference (and to allow for the selection of the feature). Their display can be modified by editing the datum and dragging the handles.
Placement Face:
Datum planes are commonly used as placement faces for sketches and other features. By building features on a datum plane, you can easily relocate an entire group of features by modifying the parameters of the datum. A datum plane is also ideal as a placement face when there is no planar face available for a feature or sketch.
Datum planes are commonly used as placement faces for sketches and other features.

A fixed datum plane (or coordinate system with components) makes a good placement face for the first sketch of a model. This datum plane can then serve as a common reference for several sketches and features in the model.

Relative datum planes can simplify your model by taking advantage of the parent-child relationship of the plane to other features.



For example, the datum plane in the figure is associated to the cylindrical face in the center of the model. A sketch and several other features are built on this datum to develop an outlet to the water pump. Merely editing the angle of the datum plane can then relocate the entire outlet. 

Another indispensable method of using a datum plane as a placement face is for creating features on a non-planar face. Features such as Hole and Slot require that the placement face be planar. For a model of a shaft, the features cannot be placed directly on the cylindrical face. However, you can create a datum plane tangent to the face then use the datum plane as the placement face.



Reference Direction:
You can use datum features to define the reference direction of a feature such as a horizontal reference for a slot feature. This is useful in cases where an edge is not available. In addition to datum axes, you can use datum planes for this purpose. The selected datum plane can intersect with the placement face to define the direction vector.



Positioning:
Using datum planes to position features offers several advantages:
- It can be quick and easy.
- You can position several features to a common datum plane.
- You can center features by positioning to a center datum plane. 




The following dimension types all allow the selection of datum planes as target objects:
 Perpendicular 
 Parallel at a Distance 
 Point onto Line 
 Line onto Line 
 Angular


Swept Features:
You can use datum planes when creating swept features. Selecting one for the Trim To Face/Plane or Trim Between Two Faces/Planes method allows you to easily edit the swept feature by moving the plane.



In the figure, we extruded the sketch and trimmed it to the datum planes. If the datum plane offset changes, the extrusion stays trimmed to the new datum plane location.

Assemblies:
Reference features can also be useful in assemblies. There may not be any suitable faces or edges to use in mating components together. However, you may be able to easily create datum planes in the two components and then mate them.

Tips:

  • Whenever you need to select a datum plane, it is easiest if you hold the cursor over one of the plane edges to highlight the plane and then pick it.
  • If you delete a datum, any dependent features of the datum are also deleted. For example, if a datum plane is the placement face for a hole and the datum is deleted, the hole is also deleted. If you move the datum instead of deleting it, dependent features also move.
Datum Features and Design Intent:
Design intent is the ability to capture geometric conditions, dimensional relationships, and relative positions between features on your solid models. Datum features can play a huge role in capturing design intent.

Design Intent:
The ability to capture design intent is commonly referred to as parametric or variational modeling. With the robust parametric features of NX, you have to make careful decisions when creating the model in order to define the design intent and take full advantage of NX's parametric abilities. The model in the figure uses several techniques to define the design intent of the wall thickness, diametral values, location of the bosses, and spacing of the ribs on the bottom face. Reference features are used to define the design intent of many of these features.

Datum Features and Capturing Design Intent:
Datum planes and datum axes are powerful tools for capturing design intent. For example, by using datum planes to position a hole and using a datum axis to create a circular array, you can retain design intent. If the part changes, the position and definition of the array remains undisturbed.
Datum planes and datum axes are powerful tools for capturing design intent.




This figure illustrates two datum planes and a datum axis being used to capture the design intent for the positioning of a pattern of counterbore holes. The initial hole (uppermost hole in the pattern) is positioned relative to the two datum planes and then the pattern was created by instancing this hole around the datum axis. Creating the pattern in this manner ensures that if the physical size of the part changes, the pattern of holes update because they were created relative to the datum features. 


Datum axes are also useful in making circular arrays parametric to a location. Instead of specifying a point and vector, a datum axis allows you to move the array by moving the datum axis.



This figure depicts a mold cap created with the help of datum features.



Datum axes are created at the intersection of the vertical datum plane and the top and bottom faces of the block. 



Datum planes are then created through the datum axes at an angle to the faces.



These planes are then used to trim material away from the cap.



The model can then be edited by changing the offset of the vertical datum plane, or the angle of the angled ones. 



To change the design intent of a model, you may have to perform operations such as reordering.



In the figure, a solid is trimmed using a datum plane. This is TRIM BODY(3) in the Part Navigator. Since it appears after the Shell feature, the front wall has been eliminated. By reordering the Shell feature after the Trim Body feature the model now has an angled wall.


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Design Process in Injection molded parts:

Design requires careful planning during the entire process. Knowing how to use the available tools in NX is the key to creating successful designs.


Conceptualization:
Before creating your part, it's a good idea to conceptualize your design. Some designers begin with a 2-D layout or even a rough CAD model, which will be redone. Hand-drawn sketches can even be a tremendous advantage in getting started. Many good designs started as a rough sketch on a napkin.
For styled consumer products, many designers sculpt their parts out of clay or Styrofoam before ever attempting to create a CAD model. This can be useful in that you can create a mockup of your part. You can study this crude prototype to determine both how functional and moldable it is. Quite often, the most obvious molding issues are revealed at this stage. Reshaping your part to make it moldable before starting your CAD model saves valuable time.

Orienting the Part:
The idea behind conceptualizing is to determine how to approach your CAD model. Think about your part in a mold tool. What features does it have and how are they oriented? Can the part be oriented in the mold tool so that there are no undercuts?

By answering these questions, you can determine the draw direction and parting line for your part. Then you have a starting point for your CAD model.
Modeling the Basic Shape:
You typically begin your model with a primitive feature, such as a block or cylinder, or by extruding a profile.



With plastic parts, you should first concentrate on modeling the main portion of your part. That is, the overall shape of the part without the individual features. This portion of your model has a nominal, uniform thickness.

Shape your part by adding additional features. Creating sketches to define trim profiles is a good approach. You can extrude or revolve these sketches to trim the solid body.



Features such as pads, pockets and slots can also be used to help shape your part. You should already be thinking about draft. Adding Taper features while creating the model in these early stages saves you time when you must prepare your model for tool design.

Adding features or extruding sketches may not always define the desired shape. You may find it necessary to create sheet bodies or additional solid bodies. Doing this allows more flexibility in the way you can define the necessary shape. These bodies are commonly referred to as tools. Use these tools to trim or subtract material away from your solid body.



You also need to be thinking about blends. Use this feature to eliminate the sharp corners of your model. Blends are normally added after Taper features. It is nearly impossible to add draft to a model using a blended Taper feature.


By concentrating on only the basic shape of the part, you can now use the Hollow feature to easily give the part a nominal, uniform thickness.


Adding Features:
Now you can begin adding features such as snaps, ribs, and bosses. The reason for holding off on these features until now is that they typically have a thickness smaller than the nominal thickness. The Hollow feature is used to define the nominal thickness, so these features should be added after the Hollow feature.



Evaluating the Design:
Once you have completed your model, you need to check it. You can use operations such as Analysis | Distance to verify the thickness in different areas. Doing this gives you a chance to catch anything you might have missed. Correcting thickness problems allows you to avoid having to deal with sink marks after the part has started a test production run.

Face Analysis on the Analyze Shape toolbar is another key tool for analyzing your part. This allows you to graphically note the draft angles. 
It can be quite easy to forget to taper some faces of your model.


Identifying problem areas on your model is an important step in the design process. Once a mold tool is cut, it can be quite expensive to modify. Carefully scrutinizing your design can easily save thousands of dollars.
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