In this tip we will show you how to maximize top down design in Pro/ENGINEER while creating the layout of a tension device. The assembly consists of a hydraulic cylinder, several linkage parts, and a roller assembly.

• We start the modeling process by creating an assembly using an std. template:

Name it top-level.asm;

Next create a skeleton model inside the top-level.asm;

Select the create a component in assembly icon to create a new part in the current assembly;

Select Skeleton Model, accept the default name:

• Use the “Copy From Existing” method and select your company start part to use as your skeleton template. If you don’t have a start part, then create one by using the Pro/ENGINEER default template. You can then browse to this part and use it as your “Copy From” option.

• Next, RMB on the TOP-LEVEL_SKEL.PRT and open it in its own window. Here we will create the layout of our linkage system. This is similar to laying out your linkages in a 2D package.

• Next, create three points for the ground locations, these points will be representative of points that do not move. They can be optimized later in the process through the use of Pro/ENGINEER Behavioral Modeling Extension. The sketch DTM point tool is a good choice for creating these points. This feature is also found under Insert à Model Datum à Point à Sketched.

• Select a plane to sketch on and create the three points. In this example the Front plane is used as the sketch plane and the Right DTM plane is used for the Right viewing reference. (Figure 1)

Notice one point is on the default coordinate system and the other two are dimensioned:

PNT0 will be used for the location of the pin joint for the cylinder;

PNT1 will be used for the location of the “V” bracket;

PNT2 will be used for the fixed location of the roller tension link.

• Next we will sketch the following for our linkages:

“V” Bracket;

Roller tension link;

Connecting linkage from V bracket to roller tension link.

Let’s start with the V Bracket:

Create a sketch datum curve feature;

Use the same sketch plane and view reference as you did with the sketched DTM point feature, just select “use previous” button.

Steps for creating the sketch in Figure 2:

Sketch a circle w/ center on PNT1 radius value of 6”;

Toggle this to construction circle;

Sketch two center lines 22.5 degrees as shown from a vertical center line;

Create three circles 1” diameter, one on PNT1, the other two at the intersections of the 6” radius construction circle and the 22.5 degree center lines.

This sketch will represent the three hole locations for our V bracket.

• Next create the roller tension linkage sketch. Use the same sketch DTM curve feature and also use the previous sketch plane references.

Steps for creating the sketch in Figure 3:

References: select PNT2 and the center of the top-right circle created from the V bracket sketch, to snap to as sketching references.

Use the sketch point icon and create sketch points on PNT2 and the top right circle from the V bracket sketch. Sketch a 3^rd point as shown above;

Create two center lines from each of these sketched points so they intersect each other at the location of the 3^rd point as shown;

Now you can create the angular dimension scheme;

Create a circle with a diameter of 1” at 1^st Point location and another at the 3^rd Point location.

• Finally, create the last sketch of the connecting linkage from V bracket to roller tension link. Use the same sketch curve feature and also the same sketch plane as in the previous features.

Sketch a linkage as shown in Figure 4:

Steps for creating this sketch:

References: select the two existing circles as sketching references.

Create 2 circles on top of the existing circles as shown;

Create 2 larger circles radius 1”;

Create tangent lines and trim to the 1” radius circles.

• Last features to be created are datum points and axis at all centers of sketched circles.

It is important that an axis exist at all centers of each circle to be used for assembly mechanism constraints.  

Now let’s create the individual parts to be used in our assembly.

Creating the V bracket part  

• Start new part – name it V_BRACKET.PRT use default template.

• Next assemble it into our TOP-LEVEL.ASM – leave the part packaged in space. Just select the OK button. This will leave the part without any constraints (we will add them later).

Activate this part to create features in it. RMB on the V_BRACKET.PRT and Activate.

Select Insertà Shared Dataà Copy Geometry;

Select Curve Refs from the dialogue box; curve chain;

Select the 3 circles from the V bracket sketch defined earlier.

Before exiting this dialogue box select the externalize option, select confirm to externalize the feature, then select the default coordinate system from the TOP-LEVEL_SKEL.PRT and the default coordinate system from the V_BRACKET.PRT.

• Create additional features to produce the final part shown in Figure 5:

• Now edit definition on the v_bracket part and create a pin joint from axis A_6 and the corresponding axis on the top-level_skel part, select the FRONT planes for each if that is the plane that is perpendicular to your axis for the pin. (Figure 6)

Creating the Roller tension link part

Start new part – name it ROLLER_TENSION.PRT use default template;

Next assemble it into our TOP-LEVEL.ASM – leave the part packaged in space;

Just select the OK button as before;

Activate the ROLLER_TENSION.PRT;

Select Insertà Shared Data à Copy Geometry;

Select Curve Refs from the dialogue box; curve chain;

Select the two circles from the roller tension linkage sketch defined earlier.

Before exiting this dialogue box select the externalize option, select confirm to externalize the feature, then select the default coordinate system from the TOP-LEVEL_SKEL.PRT and the default coordinate system from the ROLLER_TENSION.PRT.

• Create additional features to produce the final part as shown in Figure 7.

• Now edit definition and define a pin joint connection between A_4 axis and the corresponding axis on the top-level_skel part, select the FRONT planes for each if that is the plane that is perpendicular to your axis for the pin. (Figure 8)

Creating the connecting linkage from the V bracket to the roller tension link

Start new part – name it CONNECT_LINK.PRT use default template;

Next assemble it into our TOP-LEVEL.ASM – leave the part packaged in space; Just select the OK button as before;

Activate the CONNECT_LINK.PRT;

Select Insert à Shared Data à Copy Geometry;

Select Curve Refs from the dialogue box; curve chain;

Select the two circles from the connecting linkage sketch defined earlier. Also select the outside curve of the link to use for the protrusion of the part.

Before exiting this dialogue box select the externalize option, select confirm to externalize the feature, then select the default coordinate system from the TOP-LEVEL_SKEL.PRT and the default coordinate system from the CONNECT_LINK.PRT.

• Create additional features to produce the final part. (Figure 9)

• Now re-assemble the CONNECT_LINK.PRT.  

• Edit definition on the part; select the Connect tab from the assembly constraints.

• Add a pin joint to the V_BRACKET.PRT.   

• Add a cylinder joint to the ROLLER_TENSION.PRT. (Figure 10)

• Now all we have to do is add our cylinder assembly and roller.

• Assemble the ROLLER.PRT. (Figure 11)

Insert the shaft into the ROLLER_TENSION.PRT bore;

Align the end of the shaft with the face of the ROLLER_TENSION.PRT;

Now assemble the CYLINDER.ASM with a pin joint at PNT0 of the skeleton part and a cylinder joint at the v bracket. (Figure 12)

Let’s place a driver on our cylinder slider joint to simulate the range of motion.

First we need to be in Mechanism to define a driver.

Select Applications à Mechanism;

Define a servo motor: Select Mechanism à Servo Motors à New;

Select the slider joint from the cylinder assembly;

Change the Magnitude to a Cosine function; Enter the values A=1.75 (since we need total travel to be 3.5” the amplitude is total travel divided by 2) C=3.25 this is the offset we need. This will cause the cylinder to travel from 1.5” to 5” total travel.

Now let’s set up an analysis to watch our mechanism.

• Select Mechanism à Analysis and fill in the information:

Make sure to switch type to Repeated Assembly.

Now we can output a movie to show our animation:

Select Mechanism à Playback;

Select the Play button.

Now std. VCR controls allow us to play, rewind, play frame by frame, or Capture the animation to a mpg move file.

Now we are ready to use Pro/ENGINEER Behavioral Modeling Extension to instrument our design.

We need to determine the total travel of our roller part and angular travel. So we will setup some measurement features.

Select Applications à Standard to return to Assembly;

Select the Insert an analysis icon and create a Measure à Distance;

Select the axis of the roller part and the default assembly plane (ASM_RIGHT).

Now we can capture the total travel of our roller.

• Select the insert an analysis icon again. 

This time we will create a Motion Analysis.

Select next;

Select the DISTANCE parameter;

Select Run.

This will create a graph of the total travel of our roller. Now capture the minimum and maximum values. You have to select MIN_DISTANCE & MAX_DISTANCE and turn the select Yes to store these values as feature parameters. (Figure 13)

Now we can create another analysis feature to capture the total travel.

Select the insert an analysis icon again. This time create a Relation;

Select Next;

Create the following equation: travel=MAX_DISTANCE:FID_49-MIN_DISTANCE:FID_49

Use the parameter icon to access the feature parameters of MIN & MAX DISTANCE from the previous analysis feature.

Now we can create some sensitivity studies to see how changing dimensions from our skeleton model affect our travel parameter.

Select Analysis à Sensitivity Analysis;

Select the Dimension shown in red in Figure 14: Plot the travel parameter defined earlier.

The Sensitivity Analysis feature allows you to play “what if” scenarios to see what happens to analysis parameters if model dimensions change. This will only regenerate the model through the dimension range specified and will return it to its original values. Notice that any dimension can be manipulated through a range of values, even part level feature dimensions. This is an important first step in optimizing your design. Once this study is run and a value of parameter is in the range of the study then a Feasibility/Optimization study can be conducted to achieve the required parameter.

• A Feasibility Study can be set to specify an exact travel value (Figure 15):

Since we built our assembly with references to our skeleton part we only have to go to a single source to access all the controlling dimensions for point locations, lengths of linkages, and so forth. This technique makes it easy in the design stages to optimize the design in a shorter period of time.

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