How to Import and Utilize Found Relations in NX Sketcher
Using the new sketch solver, geometric relations are automatically found and are known as found relations. Whether curves are nativity drawn or imported and added to a sketch, the solver searches for found relations the same. The relations are based on curve geometry type, , position, and count. Common relations like horizontal, vertical, tangent, coincident, point on curve, equal radius among others are automatically found when a curve is moved. The move can be based on dragging when a sketch is being developed, or be based on dimension changes. In areas where found relations are not identified, manually applied found relations or persistent relations can be added to assist the solver.
Follow below steps to learn in detail ‘How to Import and Utilize Found Relations‘ in NX Sketcher:
Step 1
Open a part file.
Step 2
Data from a DXF file must be imported and converted to a sketch for modification. To import a DXF, select File tab > Import > Autocad DXF/DWG. Navigate and select dxf_import.dxf to import. Import to should be set to Work Part and then Preview.
Select Finish when complete. (If importing a DXF is not available, continue to the next step using curves hidden on layer 100.)
Once the curves are imported, double-click open space to Fit all objects on the screen.
Step 3
The curves imported are non-history based curves or what NX calls Non-timestamp geometry. The curves must be added to a sketch.
Start by creating a new sketch on the XY plane of the Datum CSYS. The imported curves are planar and flush to the XY plane already.
When the sketch is created and active, select Add Curves command.
Step 4
Choose Select All within the Add Curve dialog to choose all curve geometry.
Select OK to complete the add. The non-timestamp curves are added to the sketch and the originals deleted. The sketch should show shading indicating closed profiles. The brown color indicates the curves are movable.
Step 5
Whether curves are manually created using traditional creation methods, or imported and added in, the sketch solver treats all curves the same. Drag the indicated curve upward. Notice how the opposite side drags upward automatically. This is because a collinear relation is automatically found as the curve is moved.
Within the same shape, drag the lower horizontal line upward approximately the same distance. Again the opposite line moves as well because of a found collinear relation.
Step 6
Next drag the indicated arc downward. As the single arc is moved, the upper arc drags along as well. The distance between the two arcs is maintained. Also for both arcs, coincidents and tangents are maintained.
After the drag, select the same arc without dragging. As a curve is selected, found relations are revealed. In this case, both an Offset Relation and Concentric Relation symbols are shown. (If dragged too low the offset relation may not appear.)
Step 7
Select ESC or choose open space to cancel the selection. Next choose an end arc of the following slot shape. As the curve is selected, the solver automatically finds several relations. Symbols are displayed on all curves related to the selected as well as the other similar shapes. In addition a green preview of a radial dimension displays.
Select the radial dimension to create the dimension, change the value from R7.5 to R10. A message appears asking if the entire sketch should be scaled since this is the first created dimension. Select No.
Again choose in space to deselect all. Equal radius relations allow the similar arcs to update to the same new .
Step 8
Another dimension will be created. Choose the bottom line and the arc center shown. (To choose the arc center hover over one of the larger arcs until a center point handle displays.)
Select the 100 dimension to create the dimension and then change the value to 115. Once the dimension is created, the main circles and arcs move together, but notice the several small circles did not move consistently. This is because there was no relation that was found to maintain the curves positions.
Step 9
Return the dimension back to 100. The small circles should return to their starting position.
Since no found relation was created, a reference circle will be added to help the solver find the appropriate relation needed. Create a circle with the same center as the large circles passing though one of the small circles. Be sure to convert the circle to a reference. (Right-click the circle to convert to a reference.)
Step 10
Before the vertical dimension is changed again. First create a diameter dimension on the outer circle shown with a value of 120.
Create another diameter dimension on the reference circle with a value of 105. The reference circle gets larger. Observe how the small circles move with the diameter change. This is because point on curve relations were found upon making the reference circle larger.
Step 11
Once again the diameter of the reference circle getting larger causes the small circles to move inconsistently. The small circles move outboard properly, but the spacing between each is inconsistent.
Undo a few times to return the diameter of the reference circle back to 85. The spacing of the small circles are back to equal spacing. (Use undo instead of manually changing the diameter back to 85.)
Step 12
To help the solver identify found relations, more geometry will be added. Lines will be used to maintain the spacing of the small circles. Start by drawing a line from arc center to arc center as shown. Again, be sure to make the line reference.
If a reference line is manually drawn for each hole, dimensions would be needed to measure and hold each lines angle to maintain the hole spacing. Instead the reference line just created will be patterned. The pattern automatically maintains angle spacing. Launch Pattern.
Step 13
Within the Pattern Curve dialog, a Circular pattern is needed. Verify the setting Create Persistent Relation is active. A persistent relation is a recorded relation the solver maintains. The pattern curve will be remembered as a pattern, and thus holds the defined parameters in memory.
Pattern the reference line using the following parameters. The Rotation Point should be the large arc center. Use the Reverse Direction as needed to generate a reference line at each small circle. OK when complete.
Step 14
Since persistent relations were created, toggle Display Persistent Relations on.
The pattern relation symbol can be seen. The persistent relations is now helping the solver understand the lines must be maintained as a pattern.
Step 15
Change the vertical dimension to 115 again, and the reference circle diameter to 105 again. This time the proper relations to move and maintain the spacing of the small circles are found.
The two other sets of small circles did not update the same since the reference geometry was not created. No need to repeat the same steps for now.
Final Step
At Last, The sketch solver automatically identifies and finds most common geometric relations. Time is saved from having to generate each individual relation. For some complex conditions, persistent relations are manually created to assist the solver. To fully define the sketch would require many more dimensions that are not necessary for this project. At this point the project is now complete.
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