location.
If you use two V-blocks to hold round parts, theoretically you get four lines of clamping contact. If I know cutting pressures will be light, I often use just one V-block and the vise jaw to apply clamping pressure. You can also use some soft material between the vise jaw and the part to avoid denting the part.
If the diameters of cylindrical parts are not precise and consistant, using a V-block to hold parts may cause them to tilt or may throw center lines off location. That’s one reason you shouldn’t always take advantage of wide-open tolerances. Tight tolerances, although not necessarily needed for the part to function, may be needed to locate and hold parts accurately for further machining.
Figure 2-12 This V-block has a relatively small “V” groove cut which is used to hold a small copper pin for additional machining. Plastic material is being used here to apply pressure to avoid denting the part.
Figure 2-13 Perishable vise jaws can be used effectively to hold parts that may be difficult to hold using other methods.
12.Use perishable vise jaws. (see Fig. 2-13)
Use perishable vise jaws as a last but effective method to hold parts. I use perishable vise jaws as a last resort for the following reasons. It’s often difficult to find a set that hasn’t been all cut up. You can always make new vise blanks, but if you leave them out, they’ll likely get used quickly. Furthermore, the appropriate nests have to be machined into them, which takes extra time.
Suggestions for Get a Grip
1.Hold parts securely and accurately.
2.Find simple ways to hold parts securely.
3.Make a fixture, if needed.
4.At the end of a CNC program that drills holes into the part, add a tap drill to drill deeper into the mounting fixture.
5.Save fixtures for future use.
6.Use a good quality angle lock milling machine vise.
7.Plan setups so you can see the cut.
8.Aim for stability in your setups.
9.Use a grinding vise for additional support.
10.Construct a set of long jaws that can be bolted to the vise.
11.Use V-blocks to hold round parts.
12.Use perishable vise jaws.
Everybody crashes, I was once told. It’s likely true. However, not all crashes are created equal. There are fender benders that may just break small tools, and then there are head on collisions that may ruin your day.
Crashes are relatively easy to avoid in CNC machines. They often occur during setup and debugging. If you can recognize high-risk situations, you’ll be in a better position to avoid them.
Before discussing the mechanics of avoiding crashes, I’d like to highlight something many of you already know: One of the most effective ways of avoiding crashes is to avoid being interrupted while programming and setting up. That’s easier said than done, of course.
Having said that, this chapter provides a set of tips that have saved me numerous times!
1.Avoid moving around too much in Handle Jog mode.
If you are not familiar with the term, Handle Jog mode allows you to move the table around manually with a CNC machine. I don’t like to do much of anything with a CNC machine in Handle Jog mode. I use Handle Jog mode mostly for the bare necessities such as edge finding, indicating, and clearing the cutter. However, Handle Jog mode can be used for some simple machining.
Occasionally I use Handle Jog mode to face the end of a bar or fly cut blocks of material. However, I generally prefer machining parts under program control. We’re only human and it is relatively easy to forget which axis and feed increment you have engaged when you start cranking the feed handle. A good habit to get into is to be cautious when you start cranking the feed handle. Turn the handle just one or two clicks to verify that the spindle is moving in the direction and feed rate you want.
2.Before running a new program, scan through the program at the machine to check for gross errors. (see Fig. 3-1)
Check the Z negative moves in a new program to see if they make sense. This is an easy and often fruitful way to avoid crashes. For example, if your first tool is a center drill and you are drilling a plate, then you know the Z negative move for the center drill should be somewhere around Z –.150. If the value in the program is something like Z –1.150, then you know right away something is wrong.
You should also scan other Z negative moves in a program for drilling, reaming, tapping, etc. The Z negative moves for those operations can be easily found within the canned cycles that execute them.
Figure 3-1 Gross Z negative errors in a program translate into gross machining errors. In this example, the center drill was mistakenly programmed to go Z–1. instead of Z–.1, which resulted in a scrapped part. Machinists should do a visual scan of a new program to check for these types of errors.
3.Perform a quick visual scan of feed rates.
If you see something like F500., and you are machining stainless, then you know right away that something is wrong, at least with the feed rate. Feed rates for machining stainless are generally in the F10. to F20. range. F500. would certainly break a cutter.
4.Perform a quick visual scan of spindle speeds. (see Fig. 3-2)
Spindle speeds are sometimes incorrectly input in a program. It is easy for a programmer to add another zero to a spindle speed by mistake. Suppose a spindle speed for a reamer was meant to be 300 RPM and the programmer adds another zero and makes it 3000 RPM. In this case, the reamer is going to get fried if you don’t catch the mistake.
Before running a program, also make sure that all tool numbers are correct and that they have the correct corresponding “H” value. (The H value calls up the tool length offset for a specific tool.) For example, in a section of programming for a specific tool, you would not want to see “T2 M06” followed by “G43 H4.” The correct programming would be “T2 M06” followed by “G43 H2.” Only after calling up T4 would you want to see G43 H4 in a program.
I’ve gotten to the point where I shy away from letting other machinists run my unproven programs because a lot of them won’t take the time to do these simple checks. Further discussion
