A basic mirror operation is provided in sketch mode where one or multiple construction lines ( Lines can also be set to Mirror but are non preferred as they may divide a face upon exiting the sketch) are set as a mirror ( defining a mirror plane ). Any subsequent sketch curve drawn is then mirrored with trims, deletions etc applying to all mirrored geometry.
Exiting the sketch with the mirror lines 'off' will not create any mirror associations when exiting the sketch.
Exiting sketch with the mirror lines 'on' creates faces with edge mirror associations and upon face pulling, produces a body with face / faces having a mirror association - this mirroring association may subsequently be set on/off - and amended in various ways as discussed below.
The following can be achieved:
ONE, TWO OR N (multi ) AXIS SYMMETRIC parts Example of 'N' show first below - the 45 degree mirror plane with simultaneous horizontal and vertical mirror planes 'on', provides an efficient method to create the 8 square holes in a square symmetrical layout from drawing just a single hole. Move one hole, Pull a face and all others symmetrically reposition.
SYMMETRIC FEATURE example showing how to add ideas to an existing Body. Original concept progressing to ideas 1 then 2 is shown in stages.
MIRRORED BODIES example showing and describing the creation and modification process with limitations.
MIRROR PLANES A visual definition is shown in the below gif.
To illustrate the dynamic and flexible nature of DSM, the example part above was developed as shown below from a basic 1 axis Mirrored sketch, then later on, a central cross was added with a second Mirror axis. Lastly, the 8 small holes with 2 additional Mirror axes added after another requirement emerged.
Each of the below examples has specific requirements to operate successfully. An explanation is given.
ONE AXIS SYMMETRIC PART
Shown below is a basic symmetric part to illustrate one axIs symmetry...
For One Axis Symmetric parts, make the mirror construction line and part as shown below.
Adding further symmetry to the Original Concept, changing it to 'Idea 1'
Add a construction line for horizontal symmetry ( mirror), set it to Mirror. Ensure the existing vertical construction line is also set to Mirror condition. Use 'Project to sketch' edges to replicate existing top tang on the lower edge. Use Line to add a new upper tang. Ensure a profile ( and it's mirror ) is made. Hide body and end sketch - making a surface. Select only one of the two profile faces - they are linked by symmetry, only one to be selected. Choose Add material and Pull up to thickness of exiting body. Note as shown, faces have 2 axis symmetry .
Adding further symmetry from 'Idea 1' to' Idea 2'
DRAW THE 45 DEG CONSTRUCTION WITH EXISTING VERTICAL AND HORIZONTAL CONSTRUCTION MIRROR SET OFF AS SHOWN ( creating a single line)
Add geometry and set dimension constraint if necessary - note any dimensions to body on sketch planes are also a constraint, refer above to the 0.7 changed to 0.9 and that solid geometry can be moved relative to mirror planes.
EXAMPLE: ' N' ( multi ) AXIS SYMMETRIC PART MODIFICATION USING LABELS
Notes. The concept was a square part with full vertical and horizontal symmetry - with an additional 45 degree mirror plane, draw a single line from the centre axis to represent the outer edge / side and 8 lines are produced.
Shown below is a basic symmetric part to illustrate N ( Multi ) axis simultaneous alterations... Alterations by Move or Pull is done in the standard way however design changes using annotation Label Driving and Label Limiting values has been shown highlighting advanced functionality.
Labels are added in an annotation plane. 3D curves, Face / Face distances , Face edge length and others are all eligible. Below illustrates the use of labels applied to virtual intersections controlling faces of a Solid Body in combination with Pull or Move commands. They can be made / used / deleted at any stage of the design process to suit the current idea / requirement and not the initial creation sketch idea. Note at label creation, associated mirror planes are highlighted.
For ANY Axis Symmetric parts, it is advised to make the mirror construction lines as shown below and NOT TO DUPLICATE ( by overdrawing with symmetry on ) coincident lines. Draw the 2D geometry, exit the sketcher and pull a single face to produce a symmetrical body.
FACES MAY BE MIRRORED ( SYMMETRICALLY ) LINKED OR UN-LINKED AT ANY TIME. THE FOLLOWING METHODS ARE AVAILABLE.
CREATING NEW FACES
TO CREATE NEW LINKED FACES ( To an existing ( full or partial symmetrical Body)
Set Sketch construction lines ( create if needed) to Mirror ON. Create geometry to define new profile - geometry drawn OFFSET ( not coincident ) to the original geometry sketch perimeter will upon the face pulling / solid combining procedure, impart a new mirroring linking. Combine Add / Remove is available.
ADDING MIRROR (SYMMETRY) ASSOCIATION / LINKING TO EXISTING FACES by overdrawing body edges in a sketch with new mirror association. Make a closed profile , exit to face and pull to body and combine.
Set Sketch construction lines ( create if needed) to Mirror ON. Draw coincident with existing non mirror faces ( use 'project to sketch' for convenience / accuracy ), when combining the resulting solids, the new coincident solid must now be the target object ( first selected solid ) - otherwise new face mirroring linking isn't recognised.
SUBTRACTING MIRROR ( SYMMETRY ) FUNCTION FROM EXISTING FACES
Done in 2 ways for PERMANENT and 1 way for TEMPORARY Face un-linking
1. PERMANENT. Use PULL if faces need a reposition. Select face / faces, PULL with Mirror ICON toggled OFF. This PERMANENTLY removes mirror association with this face / faces.
2. PERMANENT. In a sketch with construction lines mirroring set to OFF. Overdraw ( or use 'Project to Sketch' ) and form a closed matching boundary over faces for un-linking. Make face / solid and combine new coincident solid as target object ( first selected solid ) - otherwise existing face mirroring will not be un-linked.
TEMPORARY Face un-linking
Select face / faces, MOVE with Mirror ICON toggled OFF. This TEMPORILY removes mirror association with this face / faces. Toggles automatically back on.
DELETION OF FACES WITH SYMMETRY ASSOCIATIONS / LINKING
Working in Wireframe and Hidden Line mode, upon any selection, any associated face is clearly displayed. Due to the various symmetry possibilities, this is very important for indicating the associated changes.
Select by individual faces or box select / power select etc. any individual or multiple symmetrical protrusions / depressions ( or holes) and delete.
Note a partial deletion of ' symmetrical features ' does not affect symmetrical behaviour of the remaining as shown in the below example. Shown is the partial top holes of the 3 axis central group is deleted with partial outer 2 axis group. No affect upon remaining associations / linking.
REMOVAL / DELETION / TEMPORARY SUSPENSION OF ANY OR ALL FACE ASSOCIATIONS ( UN-LINKING ) - 4 EXAMPLES SHOWN BELOW
1. ANY. Select the face / protrusion / depression etc, Cut and Paste, combine back to owning body - all cut /pasted faces only have associations un-linked.
2a. ANY. Select the face , select the mirror flag icon ( to un associate ) on the mirror plane and pull to position - permanently un associates the face. Note with multiple mirror planes, any associated and connected face that change size with the pull will also loose any face association.
2b. ANY. Temporary Suspension with revised subsequent associated faces. Select any face and another of it's associated faces, select the mirror flag icon ( to un associate any others) on the mirror plane and pull to position. A new association has been made on these faces.
3. ALL. Select an associated face to display the relevant MIRROR PLANE, select the Mirror plane and re select the face to deselect it - Delete. All associated faces to that mirror direction ( irrespective of creation process ) are un-linked. Delete all MIRROR PLANES to un-link all.
Example below of '1. ANY'. Deletion / Removal Face associations using Cut and Paste with Combine
Example below of ' 2a. ANY '. Pulling with mirror flag checked to un-associate permanently
Example below of ' 2b. ANY '. Temporary Suspension with revised subsequent associated faces - note the vertical mirror plane also subsequently is not showing indicating no other associated faces related with it.
Example below of '3. ALL'. Deletion / Removal Face Associations by Mirror Plane deletion
MIRRORED BODIES ( Handed Pair )
Note it is common to alter / add or subtract depressions or protrusions during a the design process however, only the faces created in the previous Sketch with Mirror have a mirror association.
To develop and modify parts /faces with an existing mirror association , if sub dividing a face to add or remove material through Pulling, a sketch with another mirror association is required. It is important that when exiting the sketch, active part geometry coincident and touching any curves is briefly turned off. This creates only a single face ( most importantly, not face dividing each mirror part) permitting successful subsequent pull operations on the 2 mirrored parts.
In the gif below, notice always the presence of the Mirror Place graphic for associated mirror faces only. - this appears during Selection, Pull or Move commands. Also notice face texturing of associated mirror faces - very apparent in edge display mode.
NOTE. Bodies may be moved independently ( Click the Mirror Plane graphic as shown to allow individual Body movement) and orientate to any position with full retention of Mirror associations.
NOTE ALL ADDITIONAL BODY MODICIFICATIONS OTHER THAN THE ASSOCIATED EXISTING FACES MOVING, PULLING ETC. CAN NO LONGER BE MADE. ( no common mirror creation plane ). Changes would be necessary to each body separately.
To ADD / CREATE additional mirrored parts, repeat the above. Make a sketch, create or project existing curve edges - a construction line must be made and set to Mirror.
Mirror body creation example: Gif 1-2
Gif 2. Remember, before exiting sketch, remove touching solid from display - this makes a separate surface to pull and not a body face division. Select only one face copy to pull - as shown below.
Example showing method of adding a depression into the Mirrored Pair above.
It is acknowledged some of the DSM mirror creation procedures could be more efficient and streamlined. The above 'work-around procedures, although fairly quick to do, are not obvious.
A Mirror / Symmetry dedicated 'Tool' can be found in the developer's own upgrade path: http://www.spaceclaim.com/DSM-upgrade-CAD.aspx