Using the CATIA DMU Kinematics Tools – Part 1 R. Lindeke, Ph.D ME 3230

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 ME 3230 11/10/2018

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 ME 3230 11/10/2018

Our Goal: ME 3230 11/10/2018

We Start: ME 3230 11/10/2018

To Add Links Click New Part and Product Name This Adds a New Part to the product ME 3230 11/10/2018

Rt. Clicking on the Part – chose Properties and Change Part’s Name 11/10/2018

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 ME 3230 11/10/2018

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) ME 3230 11/10/2018

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” ME 3230 11/10/2018

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 ME 3230 11/10/2018

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! ME 3230 11/10/2018

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 ME 3230 11/10/2018

Double Click Link2 in Tree – returns us to Part Design ME 3230 11/10/2018

1st construct line to link length – then 2 “end circles – then two B-Tangent Lines – then Q. Trim ME 3230 11/10/2018

After Adding Features and Q. Trimming as needed we have this image: ME 3230 11/10/2018

Pad the link sketch – reenter sketcher on the new top surface ME 3230 11/10/2018

Here we see the link completed – we continue similarly for all other links – and the coupler plate (only has holes not pins!) ME 3230 11/10/2018

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 ME 3230 11/10/2018

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) ME 3230 11/10/2018

Using Coincidence constraints for cylinders & Hole – we must get the axis to show before accepting – both parts! ME 3230 11/10/2018

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! ME 3230 11/10/2018

Eventually we make all the constraints then we will enter the DMU Kinematics Workbench ME 3230 11/10/2018

ME 3230 11/10/2018

1st: Click Assembly Constraints Conversion – to (revolute) joints here ME 3230 11/10/2018

After clicking use ‘New Mechanism’ – and give it a name: 11/10/2018

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 ME 3230 11/10/2018

If the base wasn’t fixed during assembly, you can do it now – must before Simulation! ME 3230 11/10/2018

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! ME 3230 11/10/2018

When its all set with joint commands and fixed parts we are ready ME 3230 11/10/2018

Using Simulate Icon we can run Immediate (our control) or On Request (automatic playback) 11/10/2018

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” ME 3230 11/10/2018

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 ME 3230 11/10/2018

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 ME 3230 11/10/2018