and those that do not. The latter ones are often called job shops or custom machine shops. The shops that have their own design capabilities should have no problem with the CAD/CAM convergence, if they manage it right. Many job shops take advantage of a computerized toolpath generation, but have no real need for CAD software. Still, they often face a string of obstacles to achieve the same goal.
Consider the realities. Your customer faxes you a drawing, asking for a quote. Your quote wins and you get the work. Often that faxed drawing is the only drawing you have from which to make the part. In a better scenario, the customer sends you a clean paper drawing. Or better yet, the customer sends you the drawing in the form of a disk file. Now, that is the best scenario, but — yes there are “buts” here.
As most work in the job shops is two dimensional (2D), the design is often done in CAD software such as Autocad by the customer. Shops that have CAM capabilities use a tool path development software such as Mastercam, EdgeCam, or GibbsCam. The question is how to get the drawing file into the CAM software. The ideal method is that the software reads the file in its native format. For example, the popular Mastercam can read and write Autocad DWG files directly, without a translator. If the software cannot read the native format of the original, it has to have a reliable translator.
Virtually all systems support DXF (drawing exchange file) and/or IGES (Initial Graphics Exchange Specification). DXF is quite simple and suitable only for two dimensional drawings that are composed of lines, arcs, circles, and points. IGES is more powerful and used for translation of complex three-dimensional drawings.
So what is the best approach for a small shop to take?
Consult with Your Customer
Consulting with your customer is probably the most important step. Your customer likes to know about your capabilities. In turn, you should know what the customer can offer to your shop, particularly when it comes to a drawing supplied on a disk or by email. Ask for a file format that your CAM software supports, preferably in the native format.
Understand CAD/CAM Translators
If the translator has to be used, make sure you understand its capabilities and its limitations. Poor translators may not convert the original geometry, especially when it contains complex geometry such as splines.
Train your CNC Programmer
Good CNC or CAD/CAM programmers can detect drawing flaws and mistakes, and often solve any problems quickly. They will also be able to eliminate geometry that is part of the drawing but not necessary to create the tool path. This skill might be one of the programmer’s most important skills.
Educate Your Customer
Do not be afraid to tell the customers what you expect from them. They will understand that your requests are made in the spirit of producing their part within specifications as well as efficiently.
Yes, it seems that for many reasons true CAD/CAM convergence is not a part of small job shops. At the same time, there is nothing wrong with CAD and CAM working together well in this unique environment.
 | Part Program Upgrading and Updating June 2004, updated February 2013 |
Regardless of the methods used, developing a CNC part program does take time. Whether written manually or generated with the aid of a CAD/CAM system, a part program should not be considered as completed until it is used to run a few parts and optimized. Even the best part programmers cannot always predict every condition during actual machining. It is not unusual — in fact, it is very common — to see CNC operators make changes to the program at the control. If the program is perfect, no changes would be necessary, a situation that rarely happens.
Optimizing a part program means improving it, mainly for more efficient performance, but also for other reasons, such as change in setup, use of a different tool, or even improved safety. Optimizing a program can take place at the control (usually by the CNC operator) or away from the control (usually by the CNC programmer). Two terms are often associated with a program change — program upgrading and program updating.
Program Upgrading
Program upgrading means strengthening the program, enriching it, and making it more cost effective without compromising quality of the part or safety of machining. When running several thousand parts in a batch or a job that repeats from time to time, upgrading part programs will have a profound effect on the overall cost of doing business. Shortening the cycle time by a few seconds can mean hours in overall savings. Here are some ideas that programmers and/or CNC operators can consider when upgrading an existing part program.
Programmed spindle speeds and cutting feedrates are the first items to evaluate; they require a very small intervention with virtually immediate improvement. It is a well-known fact that programmers take a rather conservative approach in this area. Another area of interest should be the clearances applied in the program — “cutting air” is never productive and should be minimized. Changing a grade of the cutting insert and increasing the feedrates also offer benefits without making major changes to the program. If the program contains various machining cycles, operators can make even more significant changes, depending on the cycle type.
One of the overall cycle time killers is excessive dwell time. The minimum dwell time is the amount of time required to complete one spindle revolution. In practice, this amount is often doubled to allow full revolution dwell at 50% of programmed spindle speed. For example, a programmed dwell time of one second for 1200 rpm spindle speed is excessive, yet often programmed. In this case, the minimum dwell required is 0.05 of a second, or 0.1 of a second in practice. For a few thousand parts, the time saving will be considerable.
Rapid motions can also shorten the cycle time. Combining two single motions into one simultaneous motion will also make the cycle time shorter; so too will making a tool change without moving to machine zero in all axes. There are other areas of upgrading that can be explored, some specific to a particular machine tool, for example, using a fewer threading passes on a CNC lathe.
Not all program upgrades can be made with the same ease as the suggestions provided here. For example, increasing the depth of cut may require a rewrite of the program code for a specific tool. Some changes can be possible only if the control system offers certain optional features. Equally important is knowing when not to upgrade. Program upgrading for a small nonrepetitive batch of parts may be counterproductive and not worth the time required to make the changes.
Program Updating
Program updating is not as common as program upgrading. It involves a change to the program due to a change in the engineering drawing. This situation occurs more frequently in companies that design and manufacture their own product. Jobs shops also experience a drawing change, often initiated by the customer or after mutual consultation with the customer. Often a single dimensional change may require a major program update. Talk to the part designer or engineer about tolerances that appear too tight. It is not unusual to find tolerances that can be opened up — we all know that the closer the tolerance, the more expensive it is to make the part. With more significant changes to the drawing, a complete program rewrite may often be required and worth the extra time.
The last, but not least, consideration is the quality and skills of the CNC programmers and the CNC machine operators. Good training combined with experience will reward every shop owner in a relatively short time. As a shop owner, try to provide your employees with quality training — it will pay off in no time.
| Lathe
|
