This article focusses on current V5 functionality and mostly, but not exclusively, upon the making, modifying, adding and deleting of symmetrical features that automatically duplicate design changes rather than the mirror duplication of a 1/2 finished part. Methods are shown using the current functionality for creating persistent symmetrical features with advice / tips on creating 'ad-hoc' mirror features / face copies, without linked face associations.
MIRRORING AND SYMMETRY - Beyond the 'Balanced Visual' appearance ...
Mirroring (or making) any face or feature, may either produce a component that 'fits' or 'functions' with another in one or more orientations, or only in a singular and unique way. If there is a necessity to have 2 components, that need to fit something in different ways / directions etc, it's usually less costly and faster all through the manufacturing process to produce 2 of the same component, that has an axis of symmetry allowing the appropriate usage in 2 different positions, than to produce a handed pair of different (mirrored or even entirely different) components , that each fit or function only in a singular position.
Mirroring / symmetry can be very useful for both External parts such as, Covers /Casing aesthetics, Left ~Right 'non handed' consumer products, and also for Internal parts, as a design creation helper for symmetrical features potentially offering 'Design for Manual Assembly' advantages of easier assembly due to multi-positional parts as compared to unique part orientation positioning, requiring more consideration / assembly time or additional design features for self or orientated alignment.
ARTICLE TOPICS AND QUICK LINKS...
- DESIGN PROGRESSION - SIMPLE PART - ADDING ADDITIONAL NEW SYMMETRICAL FEATURES
- 3 AXIS SYMMETRY WITH ADVANCED DIMENSION LABEL DRIVING
- EXAMPLES OF DESIGN CHANGE (in-depth) PRINCIPLES :
CREATING NEW FACES
- ADDING MIRROR ASSOCIATIONS TO EXISTING FACES
- SUBTRACTING MIRROR ASSOCIATIONS FROM EXISTING FACES
- TEMPORARILY SUSPENDING MIRROR ASSOCIATIONS
- DELETING FACES / FEATURES ( LINKED ) FROM OTHERS
- METHODS TO DELETE / REMOVE / SUSPEND MIRROR ASSOCIATIONS
- MIRROR BODIES (HANDED PAIR) THE CREATION PROCESS
- MIRROR BODIES - LIMITATIONS AFTER REPOSITIONING TO NEW PAIRED FACES
MANUAL MIRROR FACE / FEATURE / PART CREATION
Create a sketch and draw/select lines to be a mirror axis/axes. Draw lines, curves etc to make a closed sketch (producing a face) with a mirror line association, or for an ad-hoc unplanned idea, manually create it using the example methods shown below.
BASIC PRINCIPLES USING THE MIRROR TOOL
A basic mirror operation is provided in sketch mode where one or multiple construction lines ( Lines can also be set to Mirror however, these are non preferred, as they could 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 subsequent trims, deletions etc. applying to all mirrored geometry.
Note: Lines not producing a closed profile will not, upon exiting the sketch maintain their mirror associations.
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, a body is produced 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 THREE AXIS SYMMETRIC parts. Example of 'Three axis' shown 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 etc and all other faces 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 existing body. Note as shown, faces have 2 axis symmetry .
Adding further symmetry from 'Idea 1' to' Idea 2' Refer to notes under gif.
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. Remove / turn off Solid Body from display before exiting the sketch. PULL through (-) ONLY 1 of the faces as all these are linked together (as indicated by their face texture).
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 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 noting to segregate (or divide) as shown the whole pattern along the symmetry lines. exit the sketcher and pull a SINGLE FACE to produce a symmetrical body.
Example of a Clamshell shape
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 or coincident to the original geometry sketch perimeter, when pulled creates a new body or bodies ( if 2 faces are made - remember, select only a single face to Pull) . Original body and new bodies can be combined with either Add / Cut options with previous body faces retaining their links.
Remove / turn off Solid Body from display before exiting the sketch.
ADDING MIRROR ASSOCIATION / LINKING TO ALL EXISTING BODY FACES by overdrawing body edges in a sketch with new mirror association. Make a closed profile or profiles. Two examples shown.
Example 1. Creating a new symmetrical part from an existing model portion. See below image.
Example 2. Change an existing symmetrical part without any face associations into a fully face associated symmetrical body. Refer to below image.
Note: By Pull Adding or Subtraction ( adding / removing material ) a symmetrical face with mirror plane ON, the operation auto searches the object about the new mirror planes for any other possible face symmetries relative to it, and if found, new face linked associations are established.
- PERMANENT Face un-linking - Achieved in 3 ways A, B, C as below
- TEMPORARY Face un-linking
A. PERMANENT. Use PULL ( mirror icon off) to reposition a face to an asymmetrical position. This PERMANENTLY removes mirror association with this face. Pulling a face pair will disassociate the pair from others but their linking remains.
B. PERMANENT. Select required faces, rmb>Detach and (whilst selected) copy them (ctrl C) and delete faces. Paste back (ctrl V) and Combine.
C. 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. Original body linked faces, that are 'Not' replaced with the new body un-linked faces, will retain all their linked associations.
Select face / faces, MOVE with Mirror ICON toggled OFF. This TEMPORILY removes mirror association with this face / faces. Note the below situations when subsequently Pulling or Moving
Subsequent PULLING further retains face link association, all faces are pulled but with previous moved offset. Refer to Gif 3 below.
Subsequent MOVING (if original with subsequent singular face moved) it further retains face link association with previous moved offset. However, If the original move was a parallel and co planar face pair, then upon subsequent moving, any opposite parallel and co-planar pair will auto position across the mirror plane even if not selected.
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.
1. ANY - CUT AND PASTE ( Permanent face un-linking ) Select the face / protrusion / depression etc, Cut and Paste, combine back to owning body - all cut /pasted faces have face associations un-linked.
2. ANY - PULL Face Single ( Permanent face un-linking - Note does not apply to holes!- cut > paste and combine to un-link). 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.
3. ANY - PULL Face Pair > Parallel and Co-Planar ( Revision / Subtraction of association pairings from a larger existing group ) Pull any parallel and co-planar pair with mirror off - only the pairs linking association remains.
4. ANY - PULL Face Pair > Parallel and Opposite ( Revision / Subtraction of association pairings from a larger existing group ) Pull any parallel opposite pair with mirror off - all linking association remain but with the pull moved offset set.
5. ANY - MOVE (Temporary Suspension with linked faces ) Select the face, select the mirror flag icon ( to temporary un associate other faces) move to new position. Move same face again - with mirror (linked face) 'on' and observe its associated faces also move.
6. ALL - DELETE 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.
1. ANY - CUT AND PASTE - Example below showing Deletion / Removal Face associations using Cut and Paste with Combine
2. ANY - PULL Face Single - Example below showing mirror flag checked to un-associate permanently.
3. ANY - PULL Face Pair > Parallel and Co-Planar. Example below showing a pair of parallel and co-planar faces pulled with mirror association off. Note only the pair themselves now have a linked association and only the vertical mirror plane is displayed.
4. ANY - PULL Face Pair > Parallel and Opposite. Example below showing a pair of parallel and opposite faces pulled with mirror association off. Note , full association to previous faces is maintained but with an offset.
5. ANY - MOVE - Example below showing Temporary unlinking. Move a feature with flag checked allows an asymmetric pattern. MOVE again ( flag unchecked) and all original associated faces move by the same amount
6. ALL-DELETE - Example below showing Deletion / Removal Face Associations by deleting all three Mirror Planes
Note: A single plane deletion will only un-link its associations.
In a sketch plane, determine a position to make a mirror line. Make a initial profile on one side and close the sketch with the mirror ON to establish links. A surface (comprising 2 mirrored faces)s is placed in the structure browser under the active part or file/document name. PULL one face only will create two identical mirrored parts.
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 will have a mirror association thus all new symmetry / mirror faces require its sketch to have new mirror line.
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.
IF MOVING ONE OR BOTH BODIES OUT OF COMMON XYZ PLANES AND ALIGNMENTS, ANY ADDITIONAL BODY MIRROR MODICIFICATIONS OTHER THAN THE EXISTING ASSOCIATED FACES USING MOVING, PULLING ETC. CAN NO LONGER BE MADE EASILY because a common and co-planar mirror creation plane can not be established. The easiest solution might appear to add changes to each body separately however there still remains
The precise and thorough way (but seemingly more steps), is to retain the 'source mirror pair' separately ( with part drawing) for change convenience, then cut and paste each separate mirror body into a single part /component file ( if needed, because of design changes etc, replace it with a new modified 'cut source body' or 'cut feature'), save then import it with placement into the assembly position - saving the (each) component file will auto update the assembly.
The below infographic shows the principle to overcome the above issue of 2 bodies conjoined to a single component.
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.
The examples below shows various techniques for complex face / feature mirror duplication from an existing body - involving planes, sketch planes, move translation and rotation, curve / point projection, blending etc. the intention is to show the easily possible, however it is not an exhaustive list to cover all situations.
Presently for very complex parts with numerous irregular, angled or drafted faces, the efficient solution is to export an .stp file (The Add-On Exchange Module is required) into a third party software, mirror and convert back into DSM. Although the same is possible with the standard DSM included format .stl, it's inferior / slower than .stp due to face triangulation requiring either merging together or recreation depending upon the geometry.
For non complicated existing parts with few faces needing a mirror, the below manual creation techniques are an efficient method - subsequent move / pull operations can often be applied to both simultaneously.
It is acknowledged some of the DSM mirror creation procedures could be more efficient and streamlined. The above procedures, although fairly quick to do, are not obvious or as well documented as they should be.
A Mirror / Symmetry dedicated 'Tool' can be found in the developer's own upgrade path: http://www.spaceclaim.com/DSM-upgrade-CAD.aspx