North America's Leading Siemens PLM Partner

Designfusion Blog

More control over the tool axis in NX11.0.1

John Pearson - Wednesday, May 24, 2017

 

Two weeks ago, I had the privilege of attending a Cam Forum for Siemens PLM Software partners. A colleague and I drove down to Troy, Michigan, where we were introduced to new NX CAM functionality in NX11.0.1. We also saw some of the future enhancements coming in NX11.0.2 and beyond. Although there were many enhancements that I could discuss, there was one in particular that I found extremely useful. So rather than give a brief overview of all the enhancements, I will focus on one of my favorite enhancements. Once you’ve loaded NX11.0.1, open the help docs and view the what’s new section, if you’d like an overview of all the enhancements.

 

 

Interpolate Tool Axis Enhancements

 

Prior to NX11.0.1, if machining the part below, with the tool shown, you’d have a tool holder collision issue along the wall.

 


 

When situations like this occur, NX now provides a new Control Direction option, when using the Interpolate Vector tool axis option. To access this new option, expand the Tool Axis section, in the operation template. With the Axis option set to Interpolate Vector, click the Edit icon.

 


 

Notice the new Control Direction option under the Interpolation Method.

 


 

The U and V option retains the behavior from previous releases. The U option controls the tool axis in the U direction only. The V option controls the tool axis in the V direction only. These two options give the new behavior.

 

In this example, I’ll select the U from the Control Direction list.

 


 

Notice the two iso curves. Each iso curve contains a system defined vector at each end. Only one vector is now necessary to define the tool axis along each iso curve.

 


 

There is another new option, that allows us to select a system defined vector and tell the system not to consider it, when interpolating the tool axis. You do this by selecting the vector, and selecting the new Ignore Point check box. In this example, I first select vector 4, from the list.

 


 

Note: You may also select the vector by single-clicking in the graphics display. Double-clicking reverses the vector direction.

 

I then select the Ignore Point check box.

 


 

I repeat this step for vector 2.

 


 

Next, I select vector 3 and use the dynamic axis handle to rotate the tool about the YC axis, until the holder no longer collides with the part.

 


 

The third enhancement becomes apparent will doing this rotation. In previous releases, the tool was rotated about the tool tip resulting in the tool cutting below the part surface. The tool now rotates about the contact point and no longer violates the part. See the image below.

 


 

When I verify the tool path, I notice that the tool holder no longer collides with the part wall, but the tool axis begins tilting sooner than necessary. This is because NX tilts the tool axis continuously as it interpolates the tool axis between the two U curves.

 


 

I can add another iso curve to control how long the tool remains vertical before tilting. To do this I return to the Tool Axis section and click Edit again. In the Interpolate Vector dialog, I select the Add New Set icon.

 


 

Next, I select a point on the edge of the part, in the approximate position shown below.

 


 

This defines an additional iso curve with a vector that can be used to control the tilt of the tool. By leaving the ZC vector vertical, the tool axis will remain vertical as it approaches the wall until it reaches this curve.

 


 

This time, when I verify the tool path, the tool axis remains vertical until it reaches the added iso curve. It then begins to tilt as it approaches the next iso curve.

 


 

As you can see from this example, you can now specify either a U or V control direction and ignore system defined vectors, allowing you to interpolate the tool axis for variable axis operations along U or V iso curves, with as little as a single interpolation vector for each curve. This capability greatly simplifies the task of specifying a constant tool axis orientation along the entire U or V curve.

 

NX CAM: Eliminate wasted cutting motions on overhanging blank material

John Pearson - Thursday, July 28, 2016

 

Regular readers of our blog may recall my last NX CAM article, where I stated that many improvements to the software are missed due to lack of upgrade training. I gave several reason for this, which I’ll not repeat. If you’re interested, you can read the article: http://www.designfusion.com/designfusion_blog/nx-cam-options-for-selecting-cut-areas.

 

Continuing on the theme from that article, I’d like to highlight another recent improvement that may have been overlooked by some users. This improvement focuses on eliminating some wasted cut motions. My old boss, back in my CNC programming days, used to always remind me that machine time was more valuable than my time. It was his way of saying that he wanted us to make our programs as efficient as possible. So I was trained to always look for cutting efficiency. Perhaps that is why this enhancement caught my eye. This was introduced in NX9, so if you haven’t upgraded to NX9 or NX10, you have to do this manually. Let’s first look at the scenario.

 

I have a part to be machined, along with my defined blank geometry, as shown below.

 


 

Let’s assume that I rough out the bottom of the part first, using cavity mill.

 


 

Next I’ll want to rough out the top. I define my cavity mill operation and set the containment to use the IPW (in process workpiece). In other words, my blank becomes what was left after the last operation.

 


 

The image below shows the blank material after the bottom rough cut.

 


 

Prior to NX9, my cutting path would look like the following image.

 


 

Notice that the tool roughed the top, but it continued to cut the bottom half which had already been roughed away. In NX9 they added an enhancement which omits cuts that remove insignificant amounts of material from overhanging IPW’s. So in NX9, under the Strategy tab, you will see a new option called Cut Below Overhanging Blank.

 


 

If this is turned on, you will get the old pre-NX9 results, as shown above. If it is turned off, your path will generate as shown below.

 


 

Notice here that no cutting motions are wasted trying to remove the IPW left behind by the previous operation on the underside of the part. This could add up to some significant machine time savings for your company.

 

I will continue to highlight some of the newer NX CAM enhancements in future blog articles. But keep in mind that this is a slow way to learn about improvements. For example, had you attended an NX9 upgrade course, you would have learned this enhancement and more, almost 2 years ago. Imagine how much machine time that could have been saved; definitely enough to pay for the course and much more.

 

NX CAM: Options for selecting cut areas

John Pearson - Thursday, May 26, 2016

 

With the daily grind to meet production schedules, it is often difficult to keep up with all the changes to NX CAM software. I have spoken with many users who are basically still using methods that they learned from their first CAM course(s), despite the fact that there now exist more efficient ways of doing things. The primary reason for this is that they have not received any update training. Some companies expect the users to learn on their own, yet fail to provide time to do so. Others don’t see the value in upgrade training, or insist that their users simply don’t need it. Whatever the excuse, training always seems to be the lowest priority, until issues arise. I have even known companies who have even investigated changing software, when the far less expensive option of training would provide them with all that they need.

 

With this in mind, I thought it may be ideal to review some of the newer and more efficient ways of doing things in NX CAM. For this blog article I’d like to focus on the new options for cut area selection, added to the fixed and variable contour operations, in NX9. You can now define Cut Areas, for these operations, by selecting a seed face and bounding edges that form a closed loop.

 

Example 1 : Let’s start by looking at a simple example where I use a seed face inside a single loop. Here I have a Contour Area operation for the part you see below.

 


 

I start by selecting the Specify Cut Area option. I then use the new selection method that has been added. This method is labeled as Edge Bounded Region, and is found in the Selection Method list.

 


 

With this new option selected, all I have to do is select a seed face, as shown below.

 


 

Then I select the bounding edge as shown below.

 


 

Tip: To ensure the selection of the tangent curve, I make sure that the selection intent, on the Top Border Bar, is set to Tangent Curves .

 


 

I then click on Preview Region, and notice that I have selected this entire region with minimal mouse clicks.

 


 

Example 2: This example shows the selection of a single seed face that is found between two containment loops. Using the same part and operation as in Example 1, I start by selecting Specify Cut Area. I select the Edge Bounded Region option from the Selection Method list. This time I select the seed face shown below.

 


 

As before, I use the Tangent Curves selection intent to select the top closed loop.

 


 

I then select the bottom closed loop.

 

 


 

These two closed loops form the exterior and interior containment loops and when I select Preview Region , I am shown the selected area.

 


 

If you expand the Region Options on the Cut Area dialog, you will see 2 other options, the Traverse Interior Edges option, and the Use Tangent Edge Angle option.

 


 

The next two examples will look at these options.

 

Example 3 : Using the Traverse Interior Edges option.

 

In this example, I expand on Example 1, where I have already selected the faces as shown below.

 


 

But in this example, a boss and an additional edge blend has been added to the model.

 



 

If I use the same selection method as in Example 1, but also toggle on Traverse Interior Edges, the Preview Region shows me the following selection area.

 


 

Example 4 : Using the Use Tangent Edge Angle option.

 

In this final example, I have modified the part by removing the top edge blend. By removing the edge blend, the normal vectors between the faces now form a 30-degree angle.

 


 

I start by selecting Specify Cut Area. I select the Edge Bounded Region option from the Selection Method list. For my seed face I select the bottom face.

 


 

For the bounding edge I select the four exterior edges shown below.

 


 

Next, I toggle on the Use Tangent Edge Angle option and set the Angle Tolerance to 25.0000, as shown.

 


 

When I generate my operation, I notice that the top planar face is ignored. This is because the normal vectors between tangent faces exceed the specified 25-degree Angle Tolerance, therefore the adjacent face is not included in the cut area.

 


 

Rule: If the normal vectors between tangent faces equal or exceed the user specified Angle Tolerance, the adjacent face is not added to the contained area to be machined.

 


 

As you can see, these new options are more efficient than the previous method for selecting a cut area. And this is just one of the many new tools added in recent years. NX CAM continues to improve its technology, but it is up to you, the user, to learn about these improvements. It has been my experience that this does not happen unless the user is allowed the time to learn. The most cost effective way for users to improve is through professional training. Update and custom courses are available through either Siemens Training or through Designfusion. For more information, contact your Account Manager or contact us at info@designfusion.com.

 

 


Using a Contour Surface Area operation to do undercutting

John Pearson - Thursday, May 21, 2015

Recently I had a customer contact me with a part that he wished to undercut. He needed to use a spherical cutter, which eliminated the Groove Milling operation, since it only uses T-cutters. Not being an advanced user he was unsure how to proceed. With his company’s permission I’ve decided to utilize this opportunity and create a blog article on how to use the Contour Surface Area operation to do undercutting.


Below is the image of the part along with the faces (highlighted in orange) that need to be machined.

 

    

 

Before creating the operation I need to generate some geometry to use as Drive and Projection geometry. First I create a small cylinder, protruded through the center of the part (shown below in magenta). This cylinder will be used for my drive geometry. In other words, I will initially create my tool paths on the cylinder and then project them onto the surface of the part.

 


 

I place this cylinder on an unused layer so I can easily hide and show it as needed. Next I create a line along the axis of the cylinder (shown below in yellow).

 


 

I place this line on an unused layer so I can easily hide and show it as needed. I will use this line to help project the paths from the drive geometry onto the surface of the part.

 

I then create my parent groups. For the Geometry group, the customer had created a WORKPIECE1 that contained the part and was a child to the MCS shown below. He’d also created the spherical mill for the Tool group, also shown below.

 

    

 

Along with the predefined PROGRAM and MILL_FINISH method I now have enough information to begin the operation.

 

I select the Contour Surface Area operation and assign the parent groups as shown below.

 


 

Once in the operation, my first step is to specify the cut area.

 


 

I click on the Specify Cut Area icon and select the faces that I wish to machine, as shown below.

 


 

Next I need to define the Drive Geometry. I select the Edit icon (small wrench) in the Drive Method section.

 


 

I then select the Specify Drive Geometry icon.

 


 

I turn on the layer that contains the previously created cylinder. Select the cylinder as shown below. Remember the surface will be used to create my initial tool paths.

 


 

I click OK to return to the Dive Method dialog. I then expand this dialog and set the drive settings and tolerances as required by the customer.

 


 

I can verify the results, of my drive geometry settings, by clicking the Display icon under the Preview heading. Notice the orange surface mesh representing my drive geometry.

 


 

Once I have my drive geometry created, I return to the main operation dialog to select my projection vector. To do this I first turn off the cylinder layer and turn on the line layer previously created. I then set the Projection Vector to Away from Line, as shown below.

 


 

I’m prompted to specify the Line/Vector, so I select the line that I had previously created. By doing this I’m telling the system to project the tool paths on the cylinder away from the axis towards the surface of the part.

 


 

Next I ensure that my Tool Axis is set to +ZM Axis.

 


 

I then modify the Engage motion, to use the center point of the opening, as shown below. This ensures that any engage motion will start in the center of the part.

 


 

I then set my Retract motion to match the Engage motion.

 


 

Finally I set my feeds and speeds to the required values, and then generate the operation. Notice the resulting undercut.

 

 

 

The Contour Surface Area operation allowed me to define how I was going to machine the cut area, by defining a cylindrical drive surface and projecting it away from an axial line, onto the cut area.

 

If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAM courses. To arrange for advanced training please contact your Account Manager, or contact us at info@designfusion.com.