1. Using the CATIA DMU Kinematics Tools – Part 1
R. Lindeke, Ph.D
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2. Getting On The works starts with an Assembly Process
Each Link is Designed as a Part
Parts are Assembled using Assembly Constraints
Anchor the Base
Coincidences
Offsets & Contacts
Used to control the degrees of freedom of the various links
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3. Enter The DMU Kinematics Module
The assembly is “re-opened” in the DMU_Kinematics workspace
1st Convert the Assembly Constraints to Kinematic Joints
Accept the jointed linkage and self solve to resolve the remaining dof
Select the joint to move the part – and how it will be driven then …
This Allows Simulation – which can be run and used to generate Reruns and “Movies”
Lastly Simulate with “Laws” to generate velocity and acceleration graphs of interesting points and links
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4. Our Goal:
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5. We Start:
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6. To Add Links Click New Part and Product Name
This Adds a New Part to the product
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7. Rt. Clicking on the Part – chose Properties and Change Part’s Name
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8. Click on Z-X plane and Enter Sketcher
Open the New Part ‘in the tree’ double-clicking on the Part (in orange) opens the part design environment
Click on Z-X plane and Enter Sketcher
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9. Set Units (use Tools-options) Make a rectangle to hang the links on
Exit the Sketcher
Pad the Plate to 0.25 inch, then reenter the sketcher on the Front surface of the base plate
Add three circles (0.125” diameter) at the positions of the linkage (where link 2; 4 and 6 connect to ground)
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10. Leads to this after “Multi-padding” the 3 Circles
Multipad is “under” the pad tool Each circle was selected in turn and its specific height entered – Top 2 at 1/4” lower one at 1”
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11. We continue to add the Links and Coupler Plate
Click New Part Icon in Assembly Workbench
Expand Part entry in Product Tree
Rt. Click choose properties and name part link x
Double Click Part Name to enter Part Design
Select Z-X plane to sketch the fundamental shape
Each Link in turn and position near the assembly orientation using the same reference system
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12. Click No Here! As a new part is entered
After completing a part, I reentered the Assembly Workbench by double-clicking on the Product Name – now highlighted in Orange in product tree Then clicked New Part and the product name to add it!
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13. Working with each new link:
It is often easier to Hide (under rt. Click menu on a part name) existing parts while working on new parts
Enter Sketcher – set line lengths as constructions make two circles to mark the end of a link
Connect circles w/ “Bi-Tangent” line and quick trim the circles between the lines.
Add a circle of ‘pin diameter’ at one end
Pad the sketch (.25”)
Re-enter sketcher on one face and draw a circle (of pin diameter) on opposite end of link construction line
Pad circle to form linking pin for next component
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14. Double Click Link2 in Tree – returns us to Part Design
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15. 1st construct line to link length – then 2 “end circles – then two B-Tangent Lines – then Q. Trim
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16. After Adding Features and Q. Trimming as needed we have this image:
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17. Pad the link sketch – reenter sketcher on the new top surface
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18. Here we see the link completed – we continue similarly for all other links – and the coupler plate (only has holes not pins!)
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19. Assembling the Product
We use The Compass to position each link were it is closest to desired position (make sure the product is high-lighted before moving part!)
We use Coincident constraints for assembling pin-holes between link and plates
We use Coincident or Contact constraints to locate surface – all to remove dof’s in the assembly
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20. Notice the Compass is ‘attached’ to the link and is Green meaning we can move it! (1st doubleclick on Product to turn it orange then blue)
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21. Using Coincidence constraints for cylinders & Hole – we must get the axis to show before accepting – both parts!
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22. After Surface coincidence – make sure to “keep orientation” after all constraints are set, we can “update” using the Whirlpool Icon this will move the Parts into their constrained pose
Before updating – it is good practice to anchor the base so we keep fundamental orientation!
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23. Eventually we make all the constraints then we will enter the DMU Kinematics Workbench
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25. 1st: Click Assembly Constraints Conversion – to (revolute) joints here
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26. After clicking use ‘New Mechanism’ – and give it a name:
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27. After ok’ing title we had Unresolved pair 7/7 – to clear click Auto Create – if all is ok it will resolve them (0/7!)
Notice that the Product Tree has grown – with application -- Mechanism
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28. If the base wasn’t fixed during assembly, you can do it now – must before Simulation!
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29. Choose a joint to drive (angle driven) and set the limits of travel
Choose a joint to drive (angle driven) and set the limits of travel. Then simulate!
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30. When its all set with joint commands and fixed parts we are ready
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31. Using Simulate Icon we can run Immediate (our control) or On Request (automatic playback)
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32. Alternatively, we can do simulation from the DMU Generic Animation Simulation Icon – looks similar – here we can insert an on demand tool which can generate a “Replay or Video”
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33. After setting a motion pattern, We click Insert (rt
After setting a motion pattern, We click Insert (rt. Box) then we create a simulation for the Product Tree – the playback tools execute the Motion
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34. After Generating the Simulation…
We can compile the Simulation
To a replay for animating a view point
To a video file for playing offline
Then on to Simulation by “Laws” which we will cover in part two
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