Copyright Notice. HCL Technologies Ltd. All rights reserved. A DEFINITIVE GUIDE TO DESIGN FOR MANUFACTURING SUCCESS

Size: px
Start display at page:

Download "Copyright Notice. HCL Technologies Ltd. All rights reserved. A DEFINITIVE GUIDE TO DESIGN FOR MANUFACTURING SUCCESS"

Transcription

1 Title Subtitle

2 Copyright Notice HCL Technologies Ltd. All rights reserved. No part of this document (whether in hardcopy or electronic form) may be reproduced, stored in a retrieval system, or transmitted, in any form or by any means, electronic, mechanical, photocopying, recording, or otherwise, to any third party without the written permission of HCL Technologies Limited. HCL Technologies Limited reserves the right to change the information contained in this document without prior notice. The names or trademarks or registered trademarks used in this document are the sole property of the respective owners and are governed/ protected by the relevant trademark and copyright laws. This document is provided by HCL Technologies Limited for informational purposes only, without representation or warranty of any kind, and HCL Technologies Limited shall not be liable for errors or omissions with respect to the document. The information contained herein is provided on an AS-IS basis and to the maximum extent permitted by applicable law, HCL Technologies Limited hereby disclaims all other warranties and conditions, either express, implied or statutory, including but not limited to, any (if any) implied warranties, duties or conditions of merchantability, of fitness for a particular purpose, of accuracy or completeness of responses, of results, of workmanlike effort, of lack of viruses, and of lack of negligence, all with regard to the document. THERE IS NO WARRANTY OR CONDITION OF NON-INFRINGEMENT OF ANY INTELLECTUAL PROPERTY RIGHTS WITH REGARD TO THE DOCUMENT. IN NO EVENT WILL HCL TECHNOLOGIES LIMITED BE LIABLE TO ANY OTHER PARTY FOR LOST PROFITS, LOSS OF USE, LOSS OF DATA, OR ANY INCIDENTAL, CONSEQUENTIAL, DIRECT, INDIRECT, OR SPECIAL DAMAGES WHETHER UNDER CONTRACT, TORT, WARRANTY, OR OTHERWISE, ARISING IN ANY WAY OUT OF THIS DOCUMENT, WHETHER OR NOT SUCH PARTY HAD ADVANCE NOTICE OF THE POSSIBILITY OF SUCH DAMAGES. 2

3 Contents Wall Thickness Design Guidelines 4 Mold Wall Thickness... 5 Uniform Wall Thickness... 6 Wall Thickness Variation... 7 Ribs Design Guidelines 8 Recommended Rib Parameters... 9 Minimum Radius at Base of Ribs Draft Angle for Ribs Spacing Between two Parallel Ribs Bosses Design Guidelines 13 Minimum Radius at Base of Boss Spacing between Bosses Radius at Base of Hole in Boss Minimum Draft for Boss OD Minimum Draft for Boss ID Boss Height to OD Ratio Minimum Radius at Tip of Boss Chamfer at Top of Boss Wall Thickness of Boss Standalone Boss General Design Guidelines 24 Minimum Draft Angle Undercut Detection Sharp Corners Hole Depth to Diameter Ratio

4 Injection Molding Design Guidelines Wall Thickness Design Guidelines 4

5 Mold Wall Thickness The thickness of the mold wall depends on the spacing between various features in the plastic model. If features like ribs, bosses are placed close to each other or the walls of the parts, thin areas are created which can be hard to cool and can affect quality. If the mold wall is too thin, it is also difficult to manufacture and can also result in a lower life for the mold due to problems like hot blade creation and differential cooling. Minimum allowable mold wall thickness needs to be decided based on process and material considerations.. 5

6 Uniform Wall Thickness Non-uniform wall sections can contribute to warpage and stresses in molded parts. Sections which are too thin have a higher chance of breakage in handling, may restrict the flow of material and may trap air causing a defective part. Too heavy a wall thickness, on the other hand, will slow the curing cycle and add to material cost and increase cycle time. Generally, thinner walls are more feasible with small parts rather than with large ones. The limiting factor in wall thinness is the tendency for the plastic material in thin walls to cool and solidify before the mold is filled. The shorter the material flow, the thinner the wall can be. Walls also should be as uniform in thickness as possible to avoid warpage from uneven shrinkage. When changes in wall thickness are unavoidable, the transition should be gradual and not abrupt. 6

7 Wall Thickness Variation Wall thickness variation should be within tolerance so as to allow for smooth filling of the mold. Ideally, the wall thickness should be uniform throughout the part (equal to the nominal wall thickness). In reality, the variation is unavoidable due to requirements of functions and aesthetics. However, the amount of variation has to be minimized. Non-uniform wall thicknesses may cause uneven plastic flow and cause different parts of the part to cool at different rates. This can cause warpage toward the heavier portion of the model. If an uneven wall thickness is unavoidable, it may be necessary to provide additional cooling for the heavier sections. This increases tooling complexity and adds to production costs. In general, gradual change of 25% and 15% is acceptable in amorphous (PC, ABS, etc.) and semi crystalline (Nylons, PE, etc.) materials respectively. 7

8 Ribs Design Guidelines 8

9 Recommended Rib Parameters Ribs are used to improve melt flow into sections, like corners or a large boss and to increase stiffness of the part. The most economical way to increase stiffness of the part is by adding reinforcing ribs. Ribs should be placed on the mounds opening direction. For parts under bending, ribs should be placed perpendicular to the bending moment to achieve good stiffness. However, projections like ribs can create cavity filling, venting, and ejection problems. These problems become more troublesome for taller ribs. Ribs need to be designed in correct proportion to avoid defects such as short shots and provide the required strength. Thick and deep ribs can cause sink marks and filling problems respectively. Deep ribs can also lead to ejection problems. If ribs are too long or too wide, supporting ribs may be required. It is better to use a number of smaller ribs instead of one large rib (which can lead to voids or sink marks). Generally, the rib height is recommended to be not more than 2.5 to 3 times the nominal wall thickness. Similarly, rib thickness at its base should be around 0.4 to 0.6 times the nominal wall thickness. Example t = Nominal Wall Thickness W = Width of the Rib H = Height of the Rib T = Thickness at base of the Rib 9

10 Minimum Radius at Base of Ribs A fillet of a certain minimum radius value should be provided at the base of a rib to reduce stress. However, the radius should not be so large that it results in thick sections. The radius eliminates a sharp corner and stress concentration. Flow and cooling are also improved. Fillet radius at the base of ribs should be between 0.25 to 0.4 times the nominal wall thicknesses of the part. Example 10

11 Draft Angle for Ribs Draft angle design is an important factor when designing plastic parts. Such parts may have a greater tendency to shrink onto a core. This creates higher contact pressure on the core surface and increases friction between the core and the part, thus making ejection of the part from the mold difficult. Hence, draft angles should be designed properly to assist in part ejection. This also reduces cycle time and improves productivity. Draft angles should be used on interior or exterior walls of the part along the pulling direction. A general guideline suggests that draft angle for rib should be around 1 to 1.5 deg. Minimum draft should be 0.5 per side. Example 11

12 Spacing Between two Parallel Ribs Mold wall thickness gets affected due to spacing between various features in the plastic model. If features like ribs are placed close to each other or the walls of the parts, thin areas are created which can be hard to cool and can affect quality. If the mold wall is too thin, it is also difficult to manufacture and can also result in a lower life for the mold due to problems like hot blade creation and differential cooling. A general guideline suggests that spacing between ribs should be at least 2 times the nominal wall. Example 12

13 Bosses Design Guidelines 13

14 Minimum Radius at Base of Boss Bosses find use in many part designs as points for attachment and assembly. The most common variety consists of cylindrical projections with holes designed to receive screws, threaded inserts, or other types of fastening hardware. Under service conditions, bosses are often subjected to loadings not encountered in other sections of a component. Provide a generous radius at the base of the boss for strength and ample draft for easy part removal from the mold. A fillet of a certain minimum radius value should be provided at the base of boss to reduce stress. The intersection of the base of the boss with the nominal wall is typically stressed and stress concentration increases if no radii are provided. Also, the radius at the base of the boss should not exceed a maximum value to avoid thick sections. The radius at base of boss provides strength and ample draft for easy removal from the mold. It is recommended that the radius at the base of boss should be 0.25 to 0.5 times the nominal wall thickness.. 14

15 Spacing between Bosses When bosses are placed very close to each other, it results in creating thin areas which are hard to cool and can affect the quality and productivity. Also, if the mold wall is too thin, it is very difficult to manufacture and often results in a lower life for the mold, due to problems like hot blade creation and differential cooling. The general guide line suggests that spacing between bosses should be at least 2 times the nominal wall thickness. 15

16 Radius at Base of Hole in Boss Providing a radius on the core pin helps in avoiding a sharp corner. This not only helps molding but also reduces stress concentration. It is recommended that the radius at base of hole in boss should be 0.25 to 0.5 times the nominal wall thickness. 16

17 Minimum Draft for Boss OD An appropriate draft on the outer diameter of a boss helps easy ejection from the mold. Draft is required on the walls of boss to permit easy withdrawal from the mold. It is recommended that minimum draft on outer surface of the boss should be greater than or equal to 0.5 degree. 17

18 Minimum Draft for Boss ID Designs may require a minimum taper on the ID of a boss for proper engagement with a fastener. Draft is required on the walls of boss to permit easy withdrawal from the mold. It is recommended that minimum draft on the hole in boss should be greater than or equal to 0.25 degree. 18

19 Boss Height to OD Ratio A tall boss with the included draft will generate a material mass and thick section at the base. In addition, the core pin will be difficult to cool, can extend the cycle time and affect the cored hole dimensionally. General guidelines suggest that the height of boss should be less than 3 times of outer diameter. 19

20 Minimum Radius at Tip of Boss Bosses are features added to the nominal wall thickness of the component and are usually used to facilitate mechanical assembly. Under service conditions, bosses are often subjected to loadings not encountered in other sections of a component. A fillet of certain a minimum radius value should be provided at the tip of boss to reduce stress. 20

21 Chamfer at Top of Boss Boss should have chamfer on top. A chamfer at top of boss is good lead in for the fasteners. 21

22 Wall Thickness of Boss Wall thicknesses for bosses should be less than 60 percent of the nominal wall to minimize sinking. However, if the boss is not in a visible area, then the wall thickness can be increased to allow for increased stresses imposed by self-tapping screws. It is recommended that wall thickness of boss should be around 0.6 times of nominal wall thickness depending on the material.. 22

23 Standalone Boss Bosses and other thick sections should be cored. It is good practice to attach the boss to the sidewall. In this case the material flow is uniform and provides additional load distribution for the part. For better rigidity and material flow, the general guideline suggests that boss should be connected to nearest side wall. 23

24 General Design Guidelines 24

25 Minimum Draft Angle Draft angle design is an important factor when designing plastic parts. Because of shrinkage of plastic material, injection molded parts have a tendency to shrink onto a core. This creates higher contact pressure on the core surface and increases friction between the core and the part, thus making ejection of the part from the mold difficult. Hence, draft angles should be designed properly to assist in part ejection. This also reduces cycle time and improves productivity. Draft angles should be used on interior and exterior walls of the part along the pulling direction. It is typically recommended that the draft angle for sidewall should be at least between 0.5 to 2 degrees for inside and outside walls, although a larger angle will make it easier for part release. 25

26 Undercut Detection Undercuts should be avoided for ease of manufacturing. Undercuts typically require additional mechanisms for manufacture adding to mold cost and complexity. In addition, the part must have room to flex and deform. Clever part design or minor design concessions often can eliminate complex mechanisms for undercuts. Undercuts may require additional time for unloading molds. It is recommended that undercuts on a part should be avoided to the extent possible. 26

27 Sharp Corners Generously rounded corners provide a number of advantages. There is less stress concentration on the part and on the tool. Because of sharp corners, material flow is not smooth and tends to be difficult to fill, reduces tooling strength and causes stress concentration. Parts with radii and fillets are more economical and easier to produce, reduce chipping, simplify mold construction and add strength to molded part with good appearance. General design guideline suggests that corner radii should be at least one-half the wall thickness. It is recommended to avoid sharp corners and use generous fillets and radii whenever required. In addition inside and outside radii should have same center so as to avoid stresses during cooling as shown in following image. 27

28 Hole Depth to Diameter Ratio Core pins are used to produce holes in plastic parts. Through holes are easier to produce than blind holes which don t go through the entire part. Blind holes are created by pins that are supported at only one end; hence such pins should not be long. Longer pins will deflect more and be pushed by the pressure of the molten plastic material during molding. It is recommended that hole depth-to-diameter ratio should not be more than 2. 28