Help: My program is to long!

Heavy roughing machining

We have all as CNC operators experienced running out of program memory. CNC memory is just not very large. So we begin by deleting programs in memory until our new program fits. What if the memory is empty and there is still not enough room for our next part program? To follow is a few ideas to reduce CNC program size.

Check your program for repetitive blocks and replace these blocks with:

1.     A can cycle: All CNC machine controls have the ability to call standard MACRO’s that initiate internal code to repetitively do the same task over and over again such as drilling multiple holes and roughing an OD with multiple passes of equal depth of cut. Some examples are G81 and G73. Consult your owner’s manual for details.

2.     A custom macro: By writing your own custom MACRO utilizing the LOOP and END operators you can customize you own can cycle as described above. Your FANUC controls must be memory system B or above or this option is not available. Consult your programming manual and be very cautious to which common variables you use.

3.     A sub-program: By putting the repeated part of your code in another program it is now only necessary to position the machine correctly in the main program and then call another program (sub-program) to do the repetitive task. It is common practice to switch to incremental mode while in the sub-program and then back to absolute programming again when control is passed back to the main program. All axis movements in incremental mode must cancel each other out or a cumulative error will begin to grow. In other words; position the machine in exactly the same position you started incremental mode when you leave incremental mode.

Lengthy programs that are not repetitive:

1.     NURBS interpolation: If you are machining complex curves, CAD systems will output short line segments to generate a complex profile. This leads to poor surface quality. To create better surface finishes shorter line segments have to be used thus increasing again the length of the program. The CNC controls provides an answer for this: in your part program all you do is describe the curves using control points, control point weight and a knot vector. The CNC control calculates the axis movement from there. NURBS interpolation allows for higher feed rates and finer surface finishes.

2.    Drip feed:  All else has failed and the program is just not going to fit. By connecting to the DNC of the controls a PC can feed the controls, line-by-line, an extremely long CNC program. You will need to understand how to connect to your DNC and have the proper software to communicate with the controls. This requires much more set up than the other options and greater understanding of the machine tool on your part. Sometimes, it’s the only way.

Setting ATC tools as a group

Tool touch off

Setting tool groups is a process of setting the cutting tools in the Automatic Tool Changer in relationship to each other. In order to do this you must choose what is called the lead tool. All tools from this point forward should not be changed or removed and only adjusted through the wear offsets page.

Only in the event of a broken or new tool will any modifications be made to the geometry offsets page.

To set up a machine tool in this manner it is no different than the touch off process that is normally used except for the tool you have decided to use a the lead tool. For this tool it is necessary to make the Z-axis geometry offset 0.0 and set the work offset at Z 0.0 on your part. Now, call up each tool and set the geometry offsets in the Z-axis as you normally would. 

All tools are now set in relationship to the lead tool. From now on only set the lead tool in the work offset at Z zero. You may offset for wear in the wear offsets page.

This is a great time saver. If you have a hundred tools in the ATC they are all set. Every set up now only requires that the lead tool be set.  

It sounds wonderful right. Why isn’t everybody doing this? This process is very error prone to untrained operators and those not used to the process. If your organization decides to switch over to this process then every machine tool should conform to these rules. It is very confusing if some machines are set up this way and others are not. One tool set up incorrectly on either type of set up could spell disaster. 

Make sure that your management team is on board and every employee knows of the change. Otherwise you are asking for trouble.

FANUC's amazing Retract and Recover

Retract an Recover path

Using this very powerful option, a tool can easily be manipulated from a complex part with multiple X and Z-axis movements in order to work around obstructions in the features of the part and then follow the exact path automatically when returned to restart the machining operation from where it left off.  

This is an option and must already be installed on your controls. If it is not FANUC will charge a fee to turn the necessary parameters on.

The following basic steps must be followed in order for the tool to return properly.

Retract: 

1. Automatic operation is interrupted by pressing the feed hold button. You should let the spindle rotate a few times in order to reduce tool pressure.
2. Now press the retract button.
3. Switch the mode switch to rapid.
4. Make no more than 10 different moves UP and AWAY from the part.
5. Press the retract button until it flashes.
6. Press cycle stop.
7. Change your inserts. 

Recover:

1. Turn down your rapid over ride and your feed over ride switches. 
2. Press recover. 
3. Press Cycle Start. 
4. Turn up your feed rate slowly and let the machine follow the original path to the correct position.

Often it is thought that there is nothing you can do when a machine is in tapping mode but let it finish tapping a grit your teeth or hit emergency stop but with retract and recover you can stop tapping instantly and retract out of a hole when you press retract. The machine will rigid tap backwards out of the hole.

Operator maintenance and accountablilty

Daily maintenance log

The first line of defense to protect your most valuable investment is preventative maintenance. Downtime at any work center in your plant is costly in so many ways. First is the cost of repair but it does not stop there: loss in production, the possibility of a late delivery and inevitably this could lead to a dissatisfied or even lost customer down the line. The most costly side effect possible

Preventative maintenance should start with the operators at their machine conducting daily preventative measures by instilling ownership for the parts that they run and the machines that make those parts. It is their livelihood and it is foremost for a manager to clearly pass on an understanding of this principle.

Accountability has its place in every part of an organization. Follow the machine tool builder’s manual as a guide and construct a chart with it as a guide. It ensures that everyone does his or her job. Written documentation that is visually available for others to see is an effective way to enforce accountability.

By making machine operators accountable for the first level of preventative maintenance ensures that your investment in expensive machine tools is first and foremost. Setting up a work center specific checklist that is followed and signed by your operators daily is paramount. A simple check box to be sure that all recommended aspects are covered. Topping off oil levels, changing dirty filters and monitoring pressures and temperatures should be included for operators to initial and sign. 

Daily maintenance log

Managers should follow up at a minimum weekly to ensure operator preventative maintenance procedures have been followed correctly and efficiently. Be diligent in your efforts to support machinist and operators in their endeavor and provide positive reinforcement to support this important initiative. 

Cut faster grooves

Large flange undercut

I remember when I was machining; I used to get in an argument with a fellow machinist about metal removal rates on a lathe verses a mill. He would argue that his milling cutter had 10 inserts. I would come back saying that I had 100 horsepower and my insert was always in the material.

If you think about it… there are advantages to running more than a single insert. Applying this concept to a lathe in turning mode can increase productivity especially on grooves.

Lets think about the difficult situation where the underside of a flange has to be cut from solid material. You have only got two choices: You can plunge out the material with the widest grooving tool your machine can handle or use two opposing tools, one for the topside of the groove and then changing to a reverse tool to do the bottom side of the groove. The first option is slow and very noisy because of chatter. Every one in your shop will run for earplugs. The 2^nd option is inferior because it has to take tiny cuts due to how far the tools are sticking out from the tool post  

I’ve tried and tested every possibility known to man to solve this problem and then I read about chip thinning theory and had a engineering brainstorm. Button cutters exhibit chip thinning around .03 depth of cut.  What does this have to do with anything? For the same reason on a mill you can extend a high feed cutter out 7 times it’s diameter and still run 200 inches per minute. The cutting force is transferred axially, through the spindle instead of side-to-side reducing vibration and deflection during the cut.

In reality, we have to stick out our button cutter or prune tool as it is called on a lathe much farther than 7 times it’s cutting diameter We need further stiffening. You can only weld supporting steel to the cutter as wide as the cutter itself otherwise it will obstruct the cut. Since our prune tool holds a 3/8 button this does not allow for much backing or support.

What if we support our tool with another tool? Now we have to tools welded together with a ½” gusset in between supporting each other. A 1-½ inch wide double button cutter composed of two 3/8” button prune tool on each side with a supporting ½” spacer in the middle. Be sure to leave at least a one inch gap before the button inserts, not extending the support in the middle past this point.

There is more than extra support that is gained by welding these tools together. Now every pass that is taken in the Z-axis to remove material gets to travel 1 ½” less than the groove width. When I explain the path this tool travels to cut you will see that this is a big savings in time when converted to inches per minute.  

We all know that high feed mills travel at incredible feed rates. Since this tool follows the same principle it to will travel very fast up and down. So fast in it will scare the most hardy of operators and pile up chips like no other groover.  

Begin feeding this tool in at an angle. Always keeping .03 depth of cut. On a lathe this equates to .06 in diameter. This is accomplished by zigzagging up and down. Always moving in. A problem arises when you get to more than a ¼ depth of the button inserts. The tool no longer is chip thinning and begins to cut a very wise chip. At this point you will have to slow down the Z-axis feed .05 before it reaches the corner and then kick it back up when you change directions.  

G01 Z-11.0 X49.0 F.11

G01 Z-11.05 F.020

G01 Z-5.05 X48.94 F.11

G01 Z-5.0 F.02

…  

Yes, that is inches per revolution. Rock and roll baby. Let the chips fly. 

Large machined groove

Radial high feed milling

Single point turning

High feed milling

 

Radial high feed milling

They just don’t build them like they used to. Today, machine tool builders try to get the metal removal rate up through the spindle. Use a high surface footage insert, kick up the RPM’s and race through the part. It’s a good philosophy. It enables machine tools to be much less rigid than those of yester year. Comprising of much less casting weight, smaller motors and thinner ways equates to cheaper machines and therefore a smaller investment in tools.

It doesn’t really matter how fast you turn the spindle, these new machines built this way can never keep up with a big hogging machine made 30 years ago with twice the weight and 3 times the horsepower. You just can’t outdo a CNMG 8-series taking a 1-inch cut with a .035 feed rate.

Is there another way to fill up 3 hoppers a day? Yes, fortunately there is if you are facing off material and you have a “C” axis lathe. If you have been single pointing: it’s time to stop.

The following is a generic macro that can be edited for various diameters to really get the meat off. It uses a six-inch high feed mill and is feed in radially in a spiral pattern. It only takes .045 depth of cut but will run at 400 inches per minute. Always climb cut and do not use coolant but blow the chips off the top of the part to remove heat.

%

<MACRO-HIGH-FEED-FACE>

#539=169.5(OD DIAMETER)
#539-#539+7.0(OD CLEARANCE)
#540=124.3(ID DIAMETER)
#540=#540-7.0(ID CLEARANCE)
#541=0.045(DEPTH OF CUT)
#543=#538-#540
#542=[#543] / 8.4]*360(CALCULATE 70% ENGAGEMENT)

G17 G98
G97 S550 M3
#538=1
G94 G54 T0303
G00 X[#539]
Z0.0
G01 W-[#541] F450.
X[#540] H-[#542]
U-2.0
W1.0
G00 X[#539]
M00
...
M30

%

You can add a variable for total depth of cut and loop the program in and out remembering to change directions at the middle to continue climb cutting.

Change the values at the beginning of the program to match your print by editing =#539 etc… Be sure to include the “=” on the MDI screen.

This setup will have a very high chip removal rate and will definitely increase your production and profits

PIctures for process improvement

Set up supports

There is no doubt that humans are visual creatures therefore any where you can implement pictures in operating procedures can make improvements in the occurrence of errors, save time and ease the understanding of any document. Images are worth a thousand words and they can be read in seconds. Any document, no matter how technical or informative can be improved upon by incorporating pictures.

Time reduction on repeated set ups is a common focal point for improving efficiency. Effective and well-worded router operations remind an operator what was used for tooling and fixtures: in the case that it has been months since that set up was ran and in the case that it is a new operator unaware of process obstacles. Imagine now that your router has pictures and effective wording. No type of explanation or technical description can take the place of a well-shot photograph showing all the clamping, parallels and jack stands.

Tooling identification is another area where pictures can quickly used to identify the right tool. Who is going to remember or quickly finds a tool with the designation CXR5500-ABC3 but an image of this tool is almost instantly identified. 

Inserted milling cutters

One Christmas, I bought my wife a vacuum cleaner. I know, a household appliance for a present. Anyways, back to the story. Excited, she began to assemble the toy. I asked her if she needed the assembly instructions but she replied, “No”. After the construction process everything looked kosher but when she went to use it she realized the handle was on backwards. We all had a good laugh and then I began to look at the instructions. It was an exploded view with numbers and a corresponding explanation written in reference to the numbers. A light bulb went off and I realized this is the perfect way to describe the set up for complex parts. The machining cookbook was born and now individual recipes are written for parts in a family of sizes complete with pictures, process map and well-written descriptions.

These are just a few examples where pictures can be used as reminders, set up time reducers and the just plain old Ooops! I forgot to do that “stopper”. Use images anywhere you can!