Sheet Metal Assembly Design in PTC Pro/ENGINEER

Now there are two ways in which the assembly process can occur. These two ways are known as Top-down and the Bottom-up Approach. The top down approach looks at the assembly of the design with all the parts made in and already orientated with assembly constrains (placement constraints) in place in an .ASM file. So in other words all the parts are created in the assembly modelling and are assembled in one file. The Bottom-up Approach which is the assembly process that will be covering here is based on having multiple saved completed parts and then assembling them together on one assembly file.

Now to start creating an assembly from the Bottom-Up Approach, we start by going to New> Assembly> Design and then name the file accordingly and then click okay. Now to introduce the parts into the assembly, go to the right hand side of the toolbar and select the inserting components in the assembly. A window should appear allowing you to navigate in your system to select the .prt files required for the assembly.

Note: these are only placed in one at a time since you will need to specify the placement constraints in the assembly. Also note that you are using the unflatten sheetmetal design parts.

Once you have added the first part into the assembly, you will notice that there is a dashboard for your newly inserted model part. On the Dashboard, there is a message saying that the part that is added is not constrained to anything yet. To put in assembly constraints (placement constraints), you will need to go to the drop down list which is provide in the dashboard and select one of the following options depending on your needs.

Automatic- The program will assume the constraint for model and applies to the prt that is selected.

Mate – this option will allow for the combining of the two different parts. The mate placement constrain allows for you to make two selected  parts orientate themselves to either touch or not depending on the subtypes used.  The mate option has three other subtypes which are used but in principle very similar. The mate coincident allows for combining of two parts on a set amount of faces as the model is introduced into the assembly as it is. The mate offset will create the combined part with a offset set by the user on an aspect of the combination. The  mate orientation will allow the user to rearrange the part to a specific orientation as to be able to combine in a specific way.

Align-  this opinion allows for the faces of selected models to be aligned side by side with three different subtypes. The align offset, creates a offset specified by the user to have one of the two parts shift either forwards or backwards from the plane in which both parts are arranged. The align coincident allows the part to be aligned in the single plane based on the faces selected on the two parts. The align oriented allows for the orientation of the parts to be aligned in a single plane based on the face that are selected and the offset created by the option.

Insert- This placement constraint is used for the assembly of reoved components. Applying this constrain requires for you to select the inside face of the hole and the mating faces of the parts in which it is to be inserted to.

Coord Sys- This type of constraint aligns the two co ordinate systems of the parts and merge them into a single co ordinate system based on the x,y,z axis. Therefore the X axis of part 1 will be merge with x axis of the part 2 and so forth.

Tangent – Applied by selecting a circular face with another other plane or surface to make them orientate on the same plane.

Pnt on Line – Used for set datmun points or vertexes of the first part with the selected edge, axis or datum curve with the second part to be aligned.

Pnt on srf Similar to the pnt on line but uses the selected surface or datum plane of the second part to align with the first part.

Edges on srf- As the name suggest, to align the selected edge of the first part to the selected surface of the second part.

Fix – Fix the component as it already is orientated in the workspace. This is a full constraint in which the two components selected are locked into place.

Note: the parts themselves can be moved by using the move tab on the part dashboard. By use of the orient, translate, rotate and adjust options, the part can be moved accordingly with the mouse. Single click to choose the part and double click to place the part accordingly.

Now that the parts are oriented as specified, click the tick box on the dashboard to confirm the changes. Save the assembly once completed.

Demonstration 2:

Note: Use the parts which are saved in their original constructed forms not the flattened forms. If you have only saved the flatten forms, reopen the flatten forms undo the changes by deleting the flatting pattern function in the design tree. Once completed, save the file and ensure that there is a copy of each flatten design parts for the nesting section and also a normal copy of the design parts for the assembly.

Now at this stage in the project, we select create a new assembly by going to the new button, select assembly, design and then giving the assembly an appropriate name. Once completed add in the files, by select the button on the right hand side which says assemble parts. Select a single part that would like to start of as the base of the model. In this example, we will be using the Top/bottom faces of our design to be our base. Now note the new bar on top of the workspace and design tree. This is your assembly/ constraining bar for your part in the workspace. Use the Placement tabs to constrain the part to the co ordinate System Axis and the assembly. Note that the assembly/constraining bar indicates that the model is fully constrained.

Once completed, click confirm to finish. Now there are few ways in which you can constrain the next parts. Since that we have a relatively symmetrical design, we can use datum planes to do this. Before adding the next part, we create two datum planes in the XY- plane (ASM -TOP plane) with an offset of 7.5 inches in either direction. This allows us to to mate the planes together and be fixed in the correct position. Also create an additional datum pane from the XZ - plane (ASM - FRONT plane) with an offset of 7.29 inches. Now, add the next part into the assembly and constrain the model accordingly with datum planes using the align-constrains. Once completed, repeat the same insert and constraining functions for the rest of the design to complete the assembly. Here is an overview of the assembly process at each critical stage.

Figure 2.1- The Assembly Stages from left to right. 1) Creating the base for the Assembly process by constraining the part to the Co-ord sys. 2) adding the first bottom part by using the Alignment constrains with the assembly planes. 3) Demonstrating the mating constraint as the first side panel part is added to the assembly. 4) The completed Assembly with all the outlines of the parts highlighted.

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