ZW3D Quick Mill Enhances CNC Programming Efficiency
August 21, 2012
Does it get annoying to repeatedly define features of imported 3D models? Does rest milling cost you unnecessary extra programming time? Do containment definitions drive you crazy?
If so, then consider ZW3D, which gives CAM engineers like yourself rapid and efficient programming through the application of autofeature recognition, batch calculations, rapid rest roughingand rest finishing,and flexible containment.
Let me take you through a real case study to show you how ZW3D excels in each of these areas.
1. Automatic Feature Recognition
ZW3D’s Quick Mill module allows you to create tool paths directly from the whole part and stock. There is no need to define it manually, and so when you program Quick Mill, you do not need to select the machining area.
Here is the actual part I will use in this article; see figure 1. I’ll load it into ZW3D, and then select a roughing operation from the Quick Mill module. I’ve picked Rough Smooth Flow, and then directly selected the part and the stock as the machining feature.
Figure 1. Automatic feature recognition
Immediately, the definition of the machining feature is finished. Next, I need to define the tool and its parameters, following which I can calculate the results.
2. Batch Calculation
After defining the machining feature and other necessary aspects, such as the tool, process parameters, and so on, I can go on to calculate it. ZW3D provides a batch calculation function, so that I can go do other jobs while waiting for the calculations to finish. This feature helps you make full use of your time. Figure 2 shows the processing.
Figure 2. Batch calculation process
I’ll use this function to calculate the tool path. To do this, I go to the defined operation, right click it with my mouse, and then select Batch Calculation from the context menu. See figure 3.
Figure 3. Selecting batch calculation
The system gives me updates as it works through the calculations, as well as when it is done. See figure 4.
Figure 4. Setting up the alerts for batch calculation
While the calculations are being processed, I can go on to define the next operation, which is the tool path of the roughing operation seen in figure 5.
Figure 5. Roughing tool path
3. Rapid Rest Roughingand Rest Finishing
Thanks to the reference operation and reference tool, I don’t need to find the areas that cannot be cut by the big tool in the previous operation; through just one quick operation, the system detects the areas that need further cutting.
I’ll select another roughing operation; this time, it’ll be Offset 2D to get the rest roughing tool path.
First, I select the Offset 2D Operation from the Quick Mill module, and then under this operation I choose the Ref Op item from the tree. I select the previous rough as the reference operation, as shown by figure 6.
Figure 6. Adding the reference operation
Second, I set up the parameters, select a suitable tool (here I am using the 16mm flat end mill), and then I use the batch calculation function to perform the calculations.
The result is the restroughing tool path, as shown in figure 7.
Figure 7. Tool path of rest roughing
As for the rest finish, I’ll introduce it with containment. Let’s look at how containment works in ZW3D’s Quick Mill.
4. Convenient and Flexible Containment
Quick Mill cuts both steep and flat areas quickly, using angle limitations and user-defined limits to cutting regions. Limits and tool paths can be defined with a variety of geometry, such as curves, surfaces, and even curves with gaps.
Let me return to my example shape to get the finishing tool path on both flat area and steep areas. First, I’ll select the Z-level operation from the Quick Mill module, and then I’ll choose the whole part as the machining feature; for the tool, I’ve picked the 16 mm Ball End Mill.
Next, I go to the parameter section of the operation setup, and (a) pick Limiting Parameters, (b) choose Angular tap, (c) set the Min Angle to 10, and (d) the Max Angle to 90. This is shown in figure 8.
Figure 8. Setting the min and max angles
Finally, I go to the Display Parameter to change the color of tool path so that it is distinguished from the other operations. Calculate it, and I get a tool path that looks like the one in figure 9.
Figure 9. Tool path of the steep area
From the result I see that there are two problems that need to be solved. Firstly, some parts of the outside tool path are unnecessary. Secondly, there is too much lead in and lead out between tool paths. Fortunately, I found that in ZW3D it is easy to eliminate these problems.
First, I’ll go to the Limiting Parameter again, pick the XY tap, and then set the % Offset into 10. I’ll continue to theLead and Link Parameters to set the % Short Link Limit to 2000, and then recalculate the tool path. From this, I get a new path that looks like the one in figure 10.
Figure 10. Optimized tool path ofsteep area
Now that I have finished with the steep area, I can go on to cut the flat area.
I pick the Lace operation from the Quick Mill module, and then set up the tool and feature. Over in the parameter form, I enter the same values as I did for the Z level operation: I set the Min Angle to 0, the Max Angle to 22, calculate it, and I end up with the result shown in figure 11.
Figure 11. Tool path of the flat area
So, now the angular containment for steep and flat areas is set.
But sometimes I need to cut separate areas. In this case, I’ll need to limit the cutting area with a geometry, such as with a surface or a curve. So let’s take a look at how to get a separated limitation.
First, I’ll go to the Part option under Geometry, and right click the mouse to select Add Feature from the shortcut menu. See figure 12.
Figure 12. Defining profile features
Then I’ll select Profile and go to the graphic area pick the curves as the profile, as illustrated in figure 13.
Figure 13. Selecting a curve as the profile feature
There are too many tiny curves in this area, and so it isn’t very easy to get all of them. So, I’ll just select some.
But this means I get a profile with gaps in it. No problem. I’ll just set the type for this profile as “Contain,” as shown in figure 14.
Figure 14. Setting up the profile feature as Contain
I’ll use this contain to get a partial tool path, which just cuts in this area. I duplicate the previous Lace operation, and then set the part as the machining feature; I’ll also select the profile as containment, as shown in figure 15.
Figure 15. Adding Contain to machining feature
Then I calculate this operation, and get the tool path shown by figure 16.
Figure 16. The tool path with Contain
This shows how easily ZW3D provides convenient and flexible containment to make CNC programming faster for you.
Next I’ll apply a Rest Finishing operation, because some of the corners in this part are in need of further cutting.
To do this, I’ll pick the Offset 3D operation from the Quick Mill module, and then set up the machining feature by selecting 10 mm Ball End Mill as the tool.
I go to the parameter form, set up the process parameter, and then go to the Limiting Parameters to pick the 3D Tap, choosing the 16 mm End Mill as the reference tool. I calculate it, and get the tool path shown by figure 17.
Figure 17. Tool path of the rest finishing
ZW3D is all-in-one, affordable CAD/CAM which enables concept to finished product design in an integrated, collaborative environment. The proprietary Overdrive™ kernel delivers 3D part and assembly modeling, 2D production drawings, reverse engineering, motion simulation, mold design and integrated CNC machining, simplifying the design process from concept to completion. Experience ZW3D 2011, where the only limit is your imagination. Please go to www.zwsoft.com to download a free 30-day trial today.