Mistakes and oversights on blueprints and solid models can cause long delays and costly diversions in the manufacturing process. While most new computer assisted design software uses a 3D solid model to produce a 2D drawing file, some drafters and engineers still use strictly 2D software. Whether you are using a 2D or 3D software, avoiding common errors is essential for optimum cost and time effectiveness.
Here is an example of common blueprint oversights, and how to avoid them.
Sharp corners often increase the cost of a manufactured part, whether internal or external. To produce sharp or small internal corners on turned parts the machinist must use a tool with little or no corner radius producing a tool more prone to wear or chipping, as well as losing strength in the tool we must also slow the feedrate to maintain the required surface finish. Sharp or small internal corners in pockets in milled components also must be done with special tools increasing cost, during design consider the depth to corner radius ratio, internal corners with a depth to ratio larger than ten to one greatly reduces the rigidity of the tool prolonging machining time. Sharp external corners can also increase manufacturing cost, as the machinists can no longer use standard deburring practices and extra care must be taken to protect the corners during post machining operations. To avoid confusion and added cost consider a minimum internal corner call out and a maximum external callout in the notes.
Implied or called out there must be a reference to a critical area. Datums help the engineer convey to the manufacturer what feature of features are critical to the function of the part or assembly. It is also helpful to add overall part dimensions for easer quoting, as well as reducing errors in material ordering.
Over dimensioned features
By over dimensioning or double dimension a feature you and inadvertently decrease the amount of tolerance allowed. Review your blueprint for over defined features looking at all drawing views, if dimensions are pulled to the same feature from different edges one of them might need to be a reference dimension or deleted.
Surface finish callout
It is important to understand the cost of a finish callout. Standard machining surface finish historically was 125ra or greater, however over the years with the advancement of CNC machines and tooling we can now generate machined finished as fine as 8ra. With that being said the finer the surface finish the longer cycle time needed to produce such a fine finish as well as the time needed to separate the parts to protect from damage during post machining operations and shipping. There are features that need to have fine finishes in the case of sealing surfaces, however, consider only calling the important surfaces. Another helpful surface finish note, indicate which features are cosmetic surfaces that need extra attention i.e. polishing, graining, gritblasting or sanding. On mass produced parts, it is common to tumble debur the components in an abrasive media to produce parts with a uniform finish free from sharp edges, it is important to indicate in the drawing notes if this is an acceptable post process.
Things to consider about revision levels
Ensure your manufacturer has the latest revision level. If the manufacturer is using your solid model it is important that the revision levels of the solid and the blueprint match. When the engineer or designer makes changes to the print or solid a rev change needs to be made to avoid confusion. After a change has been made to the blueprints please provide a description of the change in the revision schedule, it is also helpful to put an annotation next to the changed feature or dimension.
Any threaded feature on a blueprint needs to be properly documented with the thread class. The class of thread describes the fit of a mating part. Forgetting the thread class can result in mating parts not fitting together. Another common thread oversight is not giving the machinist enough clearance at the bottom of a hole for the use of a tap. Taps roll or cut produce imperfect threads at the bottom of a hole because of the lead of the tap. When designing a part try to give a minimum of 3 times the diameter of the thread for clearance at the bottom of a hole. When a mating part must thread all the way to the bottom of a hole or up to a shoulder consider adding a thread relief with the minimum width of 1.5 times the pitch of the thread. The same principal applies to external threads if the threads need to go all the way to a shoulder consider adding a thread relief with the minimum width of 1.5 times the pitch of the thread.
First and foremost the manufacturer needs to know if the dimensions apply before or after plating. Make sure you include the type, class, and thickness of the plating. For parts with threads and tight tolerance holes, do the holes need to be plugged or masked during plating? Also, indicate where the parts can be racked during plating.
Quick mistake checklist:
Did you flip all of the drawing views the right way?
Are all of your dimensions on the print, block, and notes in the same units?
Did you accidentally snap a dimension to the tangent of a radius instead of the edge of the part?
Does your print have the correct block tolerances?
Does your print have a surface finish call out?
Is there a material type on the drawing?
Does the solid and the print match? Are they the same rev?
Do you have corner radius call outs?
Is all of the gd&t to the latest standard? Is it being used correctly?
Understanding some of these common issues that can arise with blueprints can help you to avoid these mistakes and save precious time and money. Always choose an experienced precision machining company, as these experts can quickly identify and help correct errors before manufacturing, and ensure a more cost-effective, higher quality result for you.