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| Tools present in operation toolbar |
Some of the operations are basically the same as you studied during the part design workbench, while others are new and somewhat unique to this workbench. Some of the tools present in the operation toolbar are Join, Healing, Untrim, Disassemble, Split, Trim, Scale etc. Let's see them one by one.
Join
Join tool can be used to make two surfaces or curves as one. By default, the option of "Check connexity" is selected, it ensures that the surfaces or the curves you are trying to join are actually connected. This is kind of a fail-safe to ensure that you do not join surfaces, or curves inadvertently that are not even connected. If you uncheck the option, it will let you join even surfaces that are not even connected i.e. it will appear as an operation by the name Join.x in the specification tree.
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| A surface in Green joined with Blue |
In addition to checking connexity, you can check if there's tangency between the surface you are joining. Add / Remove mode, lets you join to the list of surfaces that you wish to join, this proves to be useful, when you are trying to joining several surfaces at once and have inadvertently selected a surface that you did not want, so using remove mode, you can remove it. If you select the option 'Ignore erroneous elements' it will ignore the surfaces or curves that are affecting join operation.
Healing
Healing is a way to mend surfaces that may have gap between them and you wish to remove those gaps. These are generally not encountered in from-scratch designs. However, these may be frequently encountered during data conversion from one software to another or format change. The parameters that you can set are merging distance and distance objective. The merging distance refers to the distance value that you wish to target, so any gap above the value you set will be ignored and not targeted for healing. While distance objective is the maximum gap allowed between healed elements. So, ideally you should set to 0.001mm which is the minimum value that you can allow, the maximum value you can set is 0.1mm.
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| Healing gap between two surfaces |
If you set the continuity as 'Tangent', you will be able to set tangency angle and tangency objective, which work similar to the distance parameters that you set for point continuity.
Split
Split can be used to cut one element with another element. Not only can you cut surface with respect to other surface, you can also cut it with respect to a plane or curve (lying on the surface). Also, you can use the operation between curves and cut curves with respect to surfaces, planes etc. You need to select the 'Cutting element' and 'Element to cut' to perform the operation. You can use the other side option to keep the side of your choice. Using the same tool, you can split i.e. keep both sides of the result using the option "Keep both sides".
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| Split performed between surfaces |
Here, you can see how one of the surface is being split using another surface. Even though the blue surface does not intersect the green surface completely, it extrapolates to split the other surface. If needed, you can also opt for intersection computation, which will be a curve in this case.
Trim
Trim operation can be used to trim the surfaces / curves mutually, i.e. in this case both act as cutting elements and cut each other, this is different from Split where only one element acts as trimming element and other is the element that is cut. It should also be noted that using trim, you can cut a surface with surface, and curve with a curve. However, a surface cannot be cut with curve and vice-versa. So these are basic differences between trim and split.
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| Trim performed between two sketch curves using Standard and Pieces mode |
Also, there are two modes available, you can use the Standard mode for both surfaces as well as curves. However, the Pieces mode can be exclusively used for curves, this mode lets you check connexity and manifold edges and in addition, the various elements present in the curve are treated as individual elements in this case. To realize the difference, I would suggest you to try out the Trim command between a square sketch and circle using Standard as well as Pieces mode.
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| Trim performed between surfaces |
Above you can see trim operation performed using two surfaces, where both act as cutting elements and cut mutually. You can always use the Other side / next element to switch the side you wish to keep.
Untrim
A surface cut using the Split tool can be restored using Untrim tool. A common perception is that you would be able to restore a surface trimmed using this tool. However, that is not the case.
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| A surface split using ellipse curve, restored using Untrim tool |
Above you can see a surface is restored using Untrim tool. If the Create curves option is used, it will also extract the boundary edges related to the surface. You would be able to see all these curves in the specification tree.
Disassemble
The tool is particularly useful if you wish to make several curves within a sketch as independent, this will enable you to use the individual curves independently. The same tool can also be used in case several curves were used to extrude or create multiple surfaces in one go.
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| Revolved surfaces made independent and isolated using Disassemble |
In the above case, you can see that three rectangles were revolved and created surfaces as a unit. These can either be disassembled into 3 surfaces using 'Domains only' or 12 surfaces using 'All cells' as option. Likewise, if you have multiple curves in a sketch, you can disassemble them using this tool.
Boundary
Boundary tool is used to extract outline of a surface. There are options to define propagation type for edge selection i.e. point continuity, tangent continuity etc. For example, if you select tangent propagation, and select an edge of a surface, only the boundary that's tangent to that particular selected edge will selected and boundary will be extracted.
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| Boundary extracted shown in green, and limits defined using points on the edges |
Here you can see that we selected the surface amd also defined limits for boundary extraction using two points on the boundary.
Extract
Extract can be used to derive a surface of interest from a solid body or even an existing surface for other purposes. Like in other tools there are methods to define selection type using propagation methods - point propagation, tangent, curvature, no propagation.
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| Surface extracted shown in green |
Here, you can see a solid part from which the surface is being extracted. The surface being extracted is shown in green.
Extrapolate
The extrapolate tool can be used to extend a surface or curve. Using extrapolate, you can extend the curve based on its curvature or tangency. Likewise, you can extrapolate surface too using edge of the surface.
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| Curve and Surface extrapolation shown |
You can choose to specify length of the extrapolated element or can extend it upto certain element using the Type option. Continuity option was chosen as Point which extended the complete surface since the edge selected was in point continuity with all the edges of the surface.