Door Arm Rest Plastic Component Design Using CATIA V5
AIM: Door Arm Rest Plastic Component Design Using CATIA V5.
OBJECTIVE: Creating Door Arm Rest Plastic Design from given CLASS A and Draft analysis of the component.
Key Points:
- Bisecting method for generating Main Tooling axis
- Generating CLASS B surface from given CLASS A
- Generating CLASS C surface from given CLASS A
- Trimming CLASS A and CLASS C
- Generating Final trim for CLASS A, B, C surfaces
- Generating final plastic component from Surface component
- Generating draft analysis on component
- Conclusion
Tooling Axis (Bisecting Method):
Tooling Axis is an imaginary axis in which direction the tooling operation is performed. In Injection molding, the direction in which the mold is opened / closed, is called tooling direction.
The draft angle, which also plays a major role in plastic component design, is decided with reference to the main tooling axis of the component.
Bisecting method for generating Main Tooling axis of component.
- The given Input will be CLASS A Surface of the component, which we need to verify for boundary discontinuities.
- Then we can make a dummy tooling axis for reference by approximating from part geometry.
Observing component from different directions, we can assume the dummy tooling axis location. That would also help as first step of bisecting method.
The Z direction tooling axis, clears the drafts on sidewalls of the component and also top surface of the bezel. It is evident from below image that Z direction should be the Tooling axis of the given component.
3. For that we have to create an AXIS System on component to facilitate the Bisecting method for tooling axis creation. Extract a base surface and make a point of surface. Create new axis system on that point. This axis system acts as reference to create dummy and main tooling axis.
4. Now that the tooling direction is defined, we can make temporary tooling axis for the part as shown below. Taking the point as a reference, below image shows temporary tooling axis in Z direction. Taking it as a reference, we can proceed to define actual tooling axis using bisecting method.
5. Bisecting method will use reference lines created from different intersections of component with reference planes. Firstly, take intersection of component with ZX plane to get profile as a reference. Create two lines parallel to profile as shown in FIG 1. After creating two parallel lines, Create a bisecting line from those two lines FIG 2.
6. Similarly, take intersection of component with YZ plane to get profile as a reference. Create one line parallel to profile. Here as we do not have second reference for bisecting line, we can take a line passing through mid-point of profile. Draw line parallel to profile and passing through mid-point as shown.
7. As we can see in below FIG1, we have two different lines as output of intersection of the component with two different planes. Bisecting these two lines, we get our main tooling axis as output. Yellow Line in FIG 2 is Main Tooling axis.
Generating CLASS B Surface from CLASS A Surface as Input:
We are given a CLASS A surface as an input. Firstly, we have to generate CLASS B surface from given surface to generate solid component. CLASS B is generated by offsetting CLASS A surface. The critical parameter to consider is the component thickness. CLASS B is surface offset equal to part thickness.
Given CLASS A is divided into four main surfaces which will be helpful in generating CLASS B surface. Below image shows the CLASS A, and methodology to follow in next steps.
Offsetting Walls:
Avoiding fillets given here, Walls in violet colour can be divided into 3 surfaces. Each surface is extracted from CLASS A, Untrimmed and extrapolated to get the desired output. It will form the base for final CLASS B surface.
Extracting the surface highlighted in green, using “Extract” command.
After extracting the surface, Untrimmed it using “Untrim” command.
To further extend the surface, we can use “Extrapolate” command. It will extend the surface tangentially in all the directions. It will be useful in final trim of the component.
Further continue the same process to Extract, Untrimmed, Extrapolate the surfaces to form CLASS B surface. All three surfaces of wall are extracted from CLASS A input. These surfaces, after Untrimmed, Extrapolated, shown below.
Now that we have walls, we can trim them together to get the output. And offset them to 2.5 mm value equal to part thickness.
Offset the base:
Similarly, we can extract wall base surface, untrimmed and extrapolate it. And offset it by 2.5 mm. Also trim it with wall output. This will give CLASS B basis for Bin walls along with base.
Offset Top surface:
We have multiple Surfaces at top of the component. We have divided them already into different patches. We will process them step by step.
Top Patch 1:
Surfaces in Yellow are considered as Top Patch 1. We will extract, untrim, extrapolate and offset them one by one. Extract the Yellow surfaces as below. Extracted surfaces are extrapolated.
We have got two surfaces that we need to offset and trim together.
Top Patch 2:
Surfaces in green are considered top patch 2. Extract them from CLASS A and proceed further.
After extrapolation, we can offset and trim them together to get final output of top patch 2.
Herer are the final outputs of Top patch 1 and Top patch 2.
Upon observing, there is a small gap between these two patches. We need an extra surface to fill the gap. For that we will use sweep command.
Connecting patch between Top patch 1 and Top patch 2:
Initially we have one small surface at top portion. Which we will extract, untrim, extrapolate and offset.
To proceed further, we will need a small profile and a curve to sweep it along the empty portion between two patches. For that we use, CLASS A edge make a point on the curve. Use this point to draw a small sketch profile which is tangent to both the edges of CLASS A.
To sweep this profile, we need a guide curve. CLASS A edges can be extracted and smooth curved to generate guide curve. And proceed with sweep command to sweep sketch profile along guide curve.
To complete the connecting curve, we use “blend” command. Top surface is split to serve accurate blend surface.
We have three different surfaces. We can Join them to complete Connecting Patch between Top patch 1 and Top patch 2. The output is offset for 2.5 mm.
Top Patch 1, Top Patch 2 and Connecting patch can be trimmed together to have final output.
Final output of top surfaces can be trimmed wrt Bin walls. And the fillets are given to complete CLASS B surface.
CLASS B surface looks as below. Fillets are given and some edges are extrapolated to facilitate final trim.
Generating CLASS C surface from CLASS A surface:
CLASS A surface is used as reference to generate CLASS C surface. We need to extract outer boundary from CLASS A surface. Extract boundary using “Multiple Extract” Command. Here we can use tangent continuity option to select appropriate edges. We have to use this command several times to extract all edges.
Here also CLASS C surface generation is divided into several parts. These surfaces are extracted, and sweep along the tooling axis with draft angle of 3°.
Similarly, we can extract and Sweep some of the surfaces as shown below.
Remaining patches are critical to sweep directly. They need to process with some other operation before they are sweep and joined with CLASS C.
Bin wall LHS Multi Section Profile 1:
Bin wall LHS profile cannot be directly sweep. For that we have extrapolated connecting surfaces and split them to generate multi section surface profile. Also, the CLASS A surface edges are extracted to serve as guide curve.
We can use “Multi Section Surface” command to generate connecting profile 1.
Bin wall LHS Multi Section Profile 2:
Following the same method, we can create Bin wall RHS side Multi Section profile 2.
To proceed further, we extract, sweep, extrapolate the side profile.
To cover the remining patch of the LHS for CLASS C, we again use Multi Section Surface command. The same way as previously, we extrapolate and split the bottom surface, extract the CLASS A edges to support as guide curve and then multi section surface is generated.
Similarly, we can create the RHS patch for CLASS C. Extrapolate and split the bottom surface, extract the CLASS A edge to support as guide curve and then multi section surface is generated.
Now as we have all the surfaces ready for CLASS C, we join them to generate final CLASS C surface.
Overall, now we have CLASS A, CLASS B and CLASS C ready to trim wrt to each other to get closed surface part.
Trimming CLASS A and CLASS C :
Trim CLASS A and CLASS C surfaces together. Output is shown below.
Generating Final Trim CLASS A, CLASS B and CLASS C :
Trim above output with respect to CLASS B surface to get surface component of arm rest.
Final Output of the surface component is shown below.
Generating final plastic component from Surface component:
Above method has given a closed surface component as output. But, for manufacturing purpose, we need to have a solid body part. For that we need to migrate to CATIA V5 part workbench.
Here, in part workbench, we need to insert new body, insert menu “Body” command. This creates a new body inside part module.
In body, we can use “Close Surface” command to convert our closed surface component to Solid body part. As the name suggests, all surfaces should be closed to get proper solid body.
Choose the command and select our surface component. It will be converted to Solid body component. One of the main points is that, it won’t convert surface part to solid body if any of the boundary is open from surface component. And the final output solid part will be as shown in image.
Generating draft analysis on component:
Draft analysis gives you the overall information about draft angles required with reference to main tooling axis of the component. While designing, we could give the draft angles to desired faces to clear the tooling direction. To evaluate given draft angles, we use draft analysis tool in CATIA V5.
Draft analysis steps.
- Material mode plays a vital role in generating draft analysis. The tool calculates draft angles required based upon material properties and behaviour during tooling operation. Not setting up, will give you a warning message.
- After setting material mode, click on “Feature Draft analysis” from Insert menu. A dialogue box will be opened.
3. Use the compass option from the box, to align the current axis system with main tooling direction. It would create draft analysis with reference to tooling axis. Carefully align the axis system with main tooling axis and click on the component anywhere to create draft analysis.
4. More over for this component, we also have side core axis which also need to analyse for draft analysis.
Conclusion:
- Created the Tooling axis using bisecting method.
- Created CLASS B and CLASS C surfaces out of given CLASS A as input.
- Generated Solid body component from closed surface part.
- Used the main tooling axis for creating draft analysis on the component.
Hence, we have successfully created CLASS B and CLASS C surfaces using given CLASS A, resulting in closed surface part. This surface part is converted to solid plastic component. Used bisecting method for main tooling direction and learnt about importance of draft angle and tooling axis for plastic manufacturing process.
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