Design automation commands
Freely available commnads
These commands are available for all installations without an option.
Command | Parameters | Explanation |
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ACTIVATEPROJ(proj_id) | proj_id: Name for project. Must conform to standar Vertex project naming rules. | Create or activate a project. |
ADD(part, rep_link, filepath) | part: reference to the part being added, May include the index (#100) rep_link: determies in which representation the part is added, and wether it is a link or not. Example: V0F adds the part in representation 0, f means it is added as linked part. V2 means the part is added as a local part in represenstation 2. filepath: if the added part is not in archive, it can be read from file path, otherwise leave empty. | Add a part to the assembly |
ADDADAPTIVE(model, subassy, repr, x, y, z, alfa, beta, gamma) | model: Model name, either in archive, or filepath subassy: Subassembly, to which this component is to be added, or empty, if added to the top level representation: Representation number, in which the added part is brought to assembly (optional) x: x-position in global coordinates (optional) y: y-position in global coordinates (optional) z: z-position in global coordinates (optional) alfa: angle around x-axis (optional) beta: angle around y-axis (optional) gamma: angle around z-axis (optional) | Add an adaptive component to the assembly. Used in conjuction with stopadaptivecomponent |
ADDGROUPBYREF(group, text, mode, X, Y, origin, angle) | group: The group file path. Defaults to shared/symbols text: The text where the group will be added. mode: The mode. +1 means destroy the text. X: The X-translation from the text, or if text is not given, in global coordinates. (optional) Y: The Y-translation from the text, or if text is not given, in global coordinates.(optional) origin: Origin of the macro, integer from 1 to 9, 5 being the middle choise (optional) angle: Angle of the macro in degrees(counterclockwise) (optional) | Adds a 2D group to drawing. usesa agiven text as bases of placement. |
ADDMEAS(view, direction, plane, location, pos, elem1. elem2, text, dimtype, height, sc, XplceElem, YplceElem, inchprec, prec) | view: Projection name direction: Direction of the dimension (free, x, y, or z) plane: Plane to which the dimension is to be added (free, xy, yz or xz) location: Location of the dimension (sometimes you need this as "-400", sometimes "400" and sometimes "+400"). pos: Relative position of the dimension in the ledger line elem1: Boundary element 1 elem2: Boundary element 2 text: Dimension text. # means dimension value dimtype: Type of dimension (distance, diameter, radius, angle) height: The height of the text sc: The scale. XplaceElem: XplaceElem YplaceElem: YplaceElem inchprec: Dimensionin precision for inches, e.g. 4 or 16 prec: Dimensionin precision, e.g. 0.01.; Enter 0.1 as default | Add a dimension to 3D -model, which can be shown also in the drawing. |
ADDNEW(name, mode, ind) | name: name of the assembly. Must conform to standard vertex model naming rules mode: mode of creation
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ind: index of the part/assembly to be created | Create an empty model to either an existing assembly or base window |
ADDPNO | Add a part number to the model | |
ADDPNO3D | (obsolete) | Locate 2D part numbers through 3d (obsolete) |
ADDPROFILE(filepath,code,x1,y1,z1,x2,y2,z2, angle) | filepath: path to profiles-library and the actual profile. May begin with $DIR_SYSTEM, $DIR_SHARED or $DIR_CUSTOM code: dimension table id for the profile x1, y1, z1: coordinates for the start point i: coordinates for the end point angle: cross-section andle counterclockwise | Adds a profile to the active assembly |
ADDSEARCHPART(part) | part: reference to the part You can also define part without knowing the name: CONNECTCONSTR(FLOORLEVEL,"PARTNAME.R(R1).L(Z):1",0) command | Adds a search part for ADDADAPTIVECOMPONENT |
ADDTABLEROW(Content,Sizes,AlignModes,CutModes) | Content: "|" separated list of cell contents Sizes: "|" separated list of cell widths, size count must match to content AlignModes: "|" separated list of align modes, OPTIONAL CutModes: "|" separated list of cut modes, OPTIONAL AlignMode: 0 = left, 1 = center, 2 = right CutMode: what to do if content does not fit into cell? 0 = just cut it, 1 = cut it and add "..." at the end, 2 = split it into multiple rows inside cell | Add a row to 2D text table. Used in conjunction with STARTTABLE and ENDTABLE. |
ADDTEXT2D(type,dim_pt1, dim_pt2, dx, dy, text_angle, height, lorg, view_name, text, reflinepoints) | type: The type of the text. dim_pt1: The dimensionpoint 1 to locate the text (optional). dim_pt2: The dimension point 2 to locate the reference line start point (optional). dx: The transformation from the reference line start point dy: The transformation from the reference line start point text_angle: The text angle. height: The height of text. lorg: The lorg of the text view_name: The view name text: The text. reflinepoints: list of x,y,z -coordinates for the reference line points (optional) | Adds text to 2d drawings |
ADDTEXTS(proj, MN, id, text_type, height, xt, yt) | projection_name: The projection name in a drawing. MN: This is just MN id: The id (same as in ATTACHTEXTS). text_type: Text type (see admin manuals). height: Text height in millimeters. xt: X-translation from macro point coordinates yt: Y-translation from macro point coordinates | Adds texts in macro points (added with ATTACHTEXTS) to a specified projection in a drawing |
ASSYCHANGEREPRE(part, representation, remove_extra_parts) | part: Reference to the existing part representation: Representation number (in format Vn, where n is ithe number) remove_extra_parts: if set to | Changes representation of a part/assy |
ATTACHTEXT(part, macroname, text, id) | part: Referenct to the part. macroname: The measure point macro (must be named to_drwg, to drwg1, ...). text: The text attached to the macro. id: The id. (same as in ADDTEXTS) | Attach texts to a part. These texts can then be added to the drawing using ADDTEXTS. |
AUTOTESTINIT(mode) | mode: 1 = command list and ui not visible 2 = UI visible | Sets the user interface mode. To be used on as a background process with Flow |
BREAKLINK(views) | views: view names (optional) | Breaks the links between model and drawing for a certain view(s) |
CALCELEM(part, mode, filename, massunit, massaccuracy, locaccuracy) | part: The part or assembly to be calculated mode: 0 = return in global coordinates 1 = return in local coordinates 2 = Add data to archive card (to drawing, eventually) filename: Name of the file where the values are written to. If omitted, values are written to user/VXTASK_DEBUG. massunit: mass calculation unit 0 = ton 1 = kg 2 = g 3 = mg massaccuracy: Accuracy of mass, how many decimals locaccuracy: Accuracy of coordinates, how many decimals in X, Y, Z | Calculates the mass properties for a part or assembly |
CHANGE(part1, part2, representation, filepat) | part1: Reference to the existing part part2: Archive name of the new part representation: Representation in format Vnf, where n = representation number, f = F, if link, empty if local filepath: Complete path to an unarchived model to be added (optional) | Changes parts or subassemblies in the active assembly |
CHANGEASSEMBLY(ref, target) | ref: Part/assy to be put to antoher place in the structure target: Reference to an existing assembly in the model | Move part or asseembly to another assembly in the model |
CHANGEPROFILE(part, filepath, dimensionset) | part: Reference to the profile part to be changed filepath: Path from folder "proflibrary" dimensionset: Dimensionset of the new part | Change a profile section to another one |
CHECKMODELS(folder, save) | folder: Folder path or a project name to scan save: 1, if models are to be saved after succesful checking, 0 otherwise | Check the model health. Open and save a folder or a project. Creates entries in VXTASK_DEBUG. |
CLOSE(save) | save: is set to 1, model will not be saved when closing | Closes the active model window |
CLOSEDRAWING(drawing) | drawing: drawing number to be closed | Closes a drawing window |
CONNECTCONSTR(constraint_name, boundary_element, assemblyconstraint) | constraint_name: Name of the constraint in the adaptive component to be added. boundary_element: Reference to the boundary element in the assembly assemblyconstraint: true = assembly constraint, false = constraint in the guide part of the adaptive component | Connect constraints between assemble parts and adaptive component. |
CONSTR(constraint, elem, alterntive1, alternative2, value, direction, closer) | constraint: The constraint tobe added: angle , coincident, concentric, distance, macrolink, parallel, perpendicular, tangent elem: Reference to part 1 and it's boundary element alternative1: Reference to part 2 and it's boundary element alternative2: Alternative reference to part 2 and it's boundary element (optional) value: numerical value for distance and angle (optional) direction: + or - for surfaces. + means surface normals point to the same direction, - not (optional) closer: 1= select alternative element, which is closer to elem. 0 = select to outer one (optional) | Add an assembly constraint to the model |
CONSTR(elem1, elem2, x,y,z,alfa,beta,gamma) | elem1: Part 1 and it's insertion point macro (in format "assemblyname/partname.R(macroname)") elem2: Part 2 and it's insertion point macro (in format "assemblyname/partname.R(macroname)") x: Translation along x-axis y: Translation along y-axis z: Translation along z-axis. alfa: Rotation around x-axis beta: Rotation around y-axis gamma: Rotation around z-axis | Position two parts using macrolink-constraint If any of the values x, y, z, a, b, g are given with “?”, it means that translation or rotation is left open, and the model can freely move along that axis. Furthermore, you can enter the initial value and leave the constraint open, using syntax “150?” as a value. |
CONSTR2 | (obsolete) | |
CONSTRSET(ref1, ref2, setname1, setname2) | ref1: Reference to part 1 ref2: Reference to part 2 setname1: Constraint set name for part 1 setname2: Constraint set name for part 2 | Locate part using pre-defined constraint sets |
COPYPASTE(0,part_name,posx, posy, posz,rotz,roty,rotx,kx,ky,kz) | part_name = part name + optional reference point macro posx,posy,posz = New place in the target coordinate system dirxx,dirxy,dirxz = Direction of the X-axis in the target coordinate system rotz,roty,rotx = Part rotation kx,ky,kz = part scaling according to coordinate axis | Copies and pastes a part to another location |
COPYVIEW(InstanceRef, DrawingName,ViewName, NewViewName, UpdateNew, X, Y, LocationType, scale) | InstanceRef: Rererence to an assembly or part, from which the drawing wil lbe opened. if empty, drawing is opened from archive DrawingName: Drawing name or file path ViewName: Name of the projectino to be copied NewViewName: Name of the projection in the new drawing UpdateNew: If 1, the new projection is to be updated X: X of the new projection in the new drawing Y: Y of the new projection in the new drawin LocationType: view_location type enum describing from which corner the projectin transformation is calculated.
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scale: Scale in which the projection is brought in, like "1:2" | Copies a projection from one drawing to another, while maintaining the update-capability |
CUTPROFILE(part, index, location_mode, pos, add_meas_points, add_insertion_points) | part: Reference to the profile to be cut index: Index of a new part, which will be created by cutting original into two location_mode:
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pos: position based on location_mode. Distance in millimeters, position as 0…1. add_meas_points: add measure point macros to both ends of the profiles add_insertion_points: add insertion point macros to both ends of the profiles | Cuts one long profile into separate given pieces |
DELATTRIB | ||
DELPARTNUMBERS(ref) | ref: reference to the parts, asseblies, of which part number it to be cleared if empty, lear all part numbers in the assembly | Remove part number attribute (PNO) from a part or assembly |
DELVIEW(view) | view: projection name to be deleted | Delete a projection from active drawing |
ENDTABLE(X,Y,ShowLines,Lorg,Height) | X: x position Y: y position ShowLines: 1 = show whole grid, 0 = don't, 2 = only box around whole table, OPTIONAL Lorg: local origin 1-9, OPTIONAL Height: text height (defines row height too), OPTIONAL | Create a 2D table on the drawing. Use in conjunction with STARTTABLE and ADDTABLEROW |
EXECUTE(program, parameters, wait) | program: path to external program to be run parameters: command line parameters to be passed to the program wait: 1, wait for completion of the program, 0, keep on going | Execure an external application or a batch script |
EXIT(save) | save: if documents open, 1 saven, 0 exits without saving | Exit vertex |
EXPLODEVIEW(view) | view: projection name to be exploded to lines | Explode projection to lines |
FILEOUT(path, mode, timestamp, line) | path: path to the file mode:
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timestamp:
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line: text to be written to the file | Writes a log file, or any other text file, line by line |
FILLADB() | - | Updates the attribute data rows from replacement array, where they are to be set with GLOBALVALUE -command. |
GLOBALVALUE(key, value) | key: nameof the replacementarray key value: value to be set into the replacement array | Set a value on the replacement array. Can be used to set text macros #KEY# to drawings etc. |
LOCATE(part, xt, yt, zt, xr, yr, zr, xscale, yscale, zscale) | part: Reference to the part or assembly to be moved. xt: Translation along X-axis yt: Translation along Y-axis zt: Translation along Z-axis xr: Rotation around X-axis from global coordinates yr: Rotation around Y-axis from global coordinates zr: Rotation around Z-axis from global coordinates xscale: Scale factor in the direction of X-axis (optional) yscale: Scale factor in the direction of Y-axis (optional) zscale: Scale factor in the direction of Z-axis (optional) | Similar way to mode parts as MOVE. Use MOVE instead of this A different way to MOVE parts. |
MEASSET(part, meassetname) | part: reference to the part. meassetname: The measure set name. | Set the dimension set of a part |
MIRROR(removeoriginal, part, plane) | removeoriginal: if set to part: A reference to the part or assembly to be mirrored, can also be /. plane: The mirror plane | Mirrors the specified part or subassembly. |
MMTOINCH(accuracy, type, remove_originals) | accuracy: The accuracy as string (For example "1", "1/8", "1/2"...). type: The type of dimensioning remove_originals: if set to | Convertes millimeter-based dimensions to inches in active drawing. For detailed parameter values, see inch conversion tool in G4. |
MOVE(part, xt, yt, zt, xr, yr, zr, xscale, yscale, zscale) | part: Reference to the part or assembly to be moved. xt: Translation along X-axis yt: Translation along Y-axis zt: Translation along Z-axis xr: Rotation around X-axis (optional) yr: Rotation around Y-axis (optional) zr: Rotation around Z-axis (optional) xscale: Scale factor in the direction of X-axis (optional) yscale: Scale factor in the direction of Y-axis (optional) zscale: Scale factor in the direction of Z-axis (optional) | Moves the specified part with translation and rotation. After moving the part, it will be fixed |
MOVEVIEW(viewname,viewx1,dim_pointx1,viewx2,dim_pointx2,viewy1,dim_pointy1,viewy2,dx,dy) | viewname: The viewname. viewx1: The viewx1 dim_pointx1:The dim_pointx1. viewx2: The viewx2. dim_pointx2: The dim_pointx2. viewy1: The viewy1. dim_pointy1: The dim_pointy1. viewy2: The viewy2. dim_pointy2: The dim_pointy2. dx: The dx. dy: The dy. | Moves the selected view to another location on the drawing, based on other projections and transformation of certain inserion point in the projection to be moved. Useful when aligning projections. |
OPEN(model, mode) | model: On of
mode: if set to 1, and openeing model from Flow, do not check out | Opens model |
OPENDRAWING(part, drawing, mode, new_drawing) | part: The part or assembly reference, from which the drawing is opened. If opening a drawin directly from Flow, enter #FLOW here. If opending a drawing from hard drive, leave empty. drawing: The drawing id in archive, Flow, or a file path mode: Mode for opening the drawing. modes can be combined like 1+2 (optional)
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new_drawing: The new drawing id in archive (optional) | Open a drawing from a local model, and update the drawing link to point to the new saved drawing |
OPENFILE(filepath) | filepath: Full path to to any vxm, vxz or vxp file | Opens an unarchived vxp, vxm and vxz file from a file path |
PNOTODWG(part, view, text, dim_pt1, dim_pt2, dx1,dy1, dx2, dy2) | part: Reference to the part view: Projection name text: Part number or text dim_pt1: Dimension point 1 dim_pt2: Dimension point 2 dx1: X-translation for part number ledger dy1: Y-translation for part number ledger dx2: X-translation for part number circle dy2: Y-translation for part number circle | Adds a part number in a drawing |
REMOVE(part) | part: Part or subassembly to remove | Removes the specified part or subassembly from the assembly |
REMOVE2(part1, part2, … ) | partn: Parts or subassemblies NOT to remove from the assembly | Removes all but the specified parts from the assembly |
REMOVEFEATURES | features: Feature types to detect
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facecount: Don't remove detected features having more than this many faces (0=unlimited) boundingbox_min: Bounding box minimum size limit for feature's faces (0=unlimited) boundingbox_max: Bounding box maximum size limit for feature's faces (0=unlimited) seedshape: Shapes of faces to use as seed faces for feature detection
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radiuslimit_min: Minimum radius limit for seed faces, valid for cylinder, cone, sphere, torus radiuslimit_max: Maximumradius limit for seed faces, valid for cylinder, cone, sphere, torus seedboxlimit_min: Minumum bounding box limit for seed faces seedboxlimit_max: Maximum bounding box limit for seed faces | Remove seelcted features from the active model |
RESTOREPARAMS(type, param) | type: What type of object is restored (optional) param: what type of parameter is reverted (optional) | Restores pre-set parameters of geometry to original settings. Must be used with SETPARAMS |
SAVE(filename, ref, mode , lightmodel , ver ) | filename: The filename to which to save to. If no extension is given, save the file in archive. ref: If only one part or subassembly is saved, this is refernce. If all. reference is “/” (optional) mode: (optional)
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lightmodel: (optional)
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ver: When exporting to SAT this defines the ACIS -version in format 700, 1600 and so on (optional) | Saves and exports the model |
SAVEDRAWING(drawing, path, setup, explode, save_version, border_layer) | drawing: The drawing id. Drawing must be open. path: File name to be exported. Extension defines the format, no extension saves to archive. setup: The setup-file for dxf, dwg... (optional) explode: Explode projections when saving.(optional) save_version: When saving you can define the save version of the drawing. For example 13.0 saves drawing as Vertex G4 version 13.(optional) border_layer: If given , you can define a layer by which the borders are updated. (optional) | Saves an open drawing in several formats. Throws and error for incorrect file names. |
SCALE(scale, slave_view, update) | scale: either the scale as number, or string “1:5”, or master projection name, where scale is copied to slave slave_view: The projection name. update: if set to | Change scale of a projection |
SET2DCONSTRMGMT(onoff) | onoff: if set to 1, 2D constraint manager will be of for the rest of the task run. | Set 2D constraint manager on or off |
SETATTRIB(part, fields, vxtype, mode) | part: Reference to the part fields: Fields in format "FIELD=VALUE;FIELD2=VALUE2..." vxtype: type of database. Defaults to 11, the standard BOM database mode: mode for overwriting. 0 = update the existing attribute database row, 1 = create a new row | Set attributes like BOM data for a specified part |
SETCOLOR(part, color) | part: Reference to the part color: Lightworks material name or Vertex palette number | Changes the visualization material of the model |
SETMEAS(reference, value) | meas: Reference to the measure. in format */assy/part.measname value: Value of a measure. | Changes a driving measure |
SETNAME(part, newname) | part: Reference to the local part newname: New name | Change the name of a local part |
SETPARAMS(object, type, settings) | object: object type, So far, only “Text” is supported. type: Object type. For example, 7 = dimensions. This number corresponds to the defaultvalues show in G4 settings in keyword textpset(7). 1 = texts added by ADDTEXTS ja ADDTEXT2D. settings you can enter are: | Sets parameters for selected objects. so far only Text is supported. |
SETSMDPARAM(part, bend_table) | part: Reference to a part tobe changed bend_table: Bending table name or parametrica language program. Must be located in "bend" -folder | Change the bending table or -formula of a part |
SETSTRPLATE(part, code) | part: Reference to the part. code: The code, must be in the database | Changes the thickness of a structured plate |
SKIPMASSCALC(mode) | mode: 0 = mass calculation is normally done when needed. 1 = all mass calculation is skipped in task run after this command. | Skip mass calculation to save time |
SOLVE(mode) | mode:
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| Solves the active assembly |
SOLVEPART() | - | When the open model is a part, solve it |
STARTTABLE() | - | Starts creation of the 2D text table. use ADDTABLEROW to add rows and ENDTABLE to create the table |
STOPADAPTIVE() | - | Stops adding an adaptive component |
TRANSLATE(database, field1, field2, layer, font, mark, mode) | database: The database name field1: The field to convert from. field2: The field to convert to layer: The layer, to which the translated text appears font: The font number in DRAFT. mark: The mark is empty by default mode: Mode = 1, is multirow texts are to be handled one row at a time, otherwise 0 | Translates the drawing with a translation database |
UPDTEXTMACROS() | - | Updates text macros in the active drawing |
UPDVIEWS() | - | Updates 3D -projections in the active drawing |
VISIBILITY(part, visibility, represenstations) | part: Reference to the part. visibility: The visibility, either "+" as visible, "-" as hidden. representations: The representations as a string, separated by a comma (E.g. "0, 2, 5"). | Changes the visibility of a part in the active model |
VISIBILITYFAST(part, visibility, represenstations) | part: Reference to the part. visibility: The visibility, either "+" as visible, "-" as hidden. representations: The representations as a string, separated by a comma (E.g. "0, 2, 5"). | Changes the visibility of a part in the active model, really fast compared to the older version |
Commands available for users with “Design automation” -option
Command | Parameters | Explanation |
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ADDITEM(child, mother, quantity) | child: Type of the object to be created: "item", "customer", "project", ... mother: Codew of mother object. Must be unique quantity: how many childs are added | Adds an item to another item's structure, requires Flow. |
BOOLEAN(parts_to_be_machined, machining_parts,action, offset, machining_parts) | parts_to_be_machined: Refernce to parts, which are to be machined. machining_parts: reference to parts, which are doing the machining. Also assemblies action:
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offset: machining offset from the machining part only_larger_remains: 1, is only larger volume remains | Boolean operators |
CLOSEDEBUGFILE() | - | Ends debug-redirect to custom file. After this debug logs goes back to ./VXTASK_DEBUG. Requires OPENDEBUGFILE -command to be used before. |
COLLECTFEATS(file) | file: path to which the features are to be saved | Collect machining features form the model. Requires Hydraulic Block Design -option. |
COLLECT_PARTLIST(assy, file, formatfile , where, rollout, kompot_choise, repstr) | assy: Reference to the assembly file: File path where the BOM will be saved formatfile: format file where: where-clause to filter the entries rollout: rollout = 1, collect from al levels kompot_choise: kompot choise, which describes the above selections. to_drawing: if set to to_database: if set to number_parts: if set to representation: representation number, from whih the BOM data is collected | Collect parts list to text file, tranfer to product database or update the bom in sheet. |
COLLISIONS() | - | Checks for any collisions in the model. Outputs to debug log file. |
COMPAREDRAWING(drawingname, leaveopen, tolerance) | drawingname: Archive name or path to a drawing to be compared to active open drawing leaveopen: If 1, leave the compared drawing as a subdrawing. In general, set to 0 tolerance: tolerance which defines the distance between points which are still considered "the same" | Compares two drawings line by line |
COMPAREFILES(pic1, pic2) | pic1: File path to vxp file 1 pic2: File path to vxp file 2 | Places two Vertex drawings on top of each other, and writes differences to VXTASK_DEBUG_file |
CONNECT(obj_type1, obj_code1, obj_type2, obj_code2) | obj_type1: Type of the first object: "item", "customer", "project", ... obj_code1: The code of the object obj_type2: Type of the second object: "item", "customer", "project", ... obj_code2: The code of the object | Connects two Flow-objects. Requires Flow. |
CREATE(filename) | filename: name of file to be created | Creates a file to the file system. Like *nix “touch”. Requires operator FILE_DIR |
CREATEPDF() | - | Creates PDF book. Requires STARTPDF -command before. |
DELETEDRAWING(id) | id: archive number of the drawing to be deleted | Deletes drawing completely from the archive. Does not ask any confirmations. |
DELETEMODEL(id) | id: archive number of the model to be deleted | Deletes model completely from the archive. Does not ask any confirmations. |
DELETEPROJ(id) | id: archive number of the project to be deleted | Deletes project completely from the archive. Does not ask any confirmations. |
DELITEM(itemcode, del_links, keep_item) | itemcode: Item code of an item to be deleted from Flow del_links:
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keep_item: 1, if the item itself is not deleted | Deletes item from Flow. Requires Flow. |
EDITPARTLINES(part, mode, viewname, layer, pen_width, sort, rsize, color) | part: Reference to a 3D part, not an assembly mode: Mode? viewname: Name of the 2D projection layer: Layer number of the lines pen_width: Line thickness sort: Line type (from lines properties) rsize: Line scale (for dot, dot-dash and so on) color: Line color | Set 2D parameters of a part’s lines. |
LOADSTUDIO(name) | name: visualization studio name | Loads a predefined studio |
MODELDATATOFILE(path, reference, skip_acis_check) | path: File path of the file to be created reference: Reference to subassembly. If empty, the top level will be used skip_acis_check: If true, does not perform ACIS-check before exporting | Save the model data to a text file |
NOMESSAGES(no_messages) | no_messages: 1=messages will not be written to VXTASK_DEBUG after this command. 0= messages will be written to VXTASK_DEBUG from this point on. | Turns off/on reporting of the commands. If set on, all command will produce messages into VXTASK_DEBUG. Useful only on slow internet connections and huge taskfiles. |
OPENDEBUGFILE(file) | file: file path | Redirect the output to a given file, unless this is used, it will be written to ./VXTASK_DEBUG. Remeber to close this with CLOSEDEBUGFILE |
PARTPLISTMODE(part, partplistmode) | part: Reference to the part. partlistmode: 0 = Archive data to parts list, 1 = Not included in parts list, 4 = set "Explode to parts list" on | Specifies how the parts are to be collected to the partslist |
PAUSE() | - | If debugfeatures are set, this function adds a "breakpoint" to active modelling |
PDMPLISTTOXML(item,fields,file) | item: iten id, where to thructure is to be collected fields: If empty, all fields will be returned. Otherwise, a smicolon-separated list of field names (e.g. UNIQUEID;PNO;OBJCODE;DESCR) file: file path to write | Item structure from Flow to XML |
POINTCLOUDSCALE(part, scale) | part: reference to the point cloud in the active model scale: new scale either as numeric or string format | Scales point could models |
POINTCLOUDTHINOUT(part, dim) | part: reference to the point cloud in the active model dim: thinout dimension | Makes thinout to point clound parts |
REMOVEDRAWING(part, drawing) | part: The part or assembly reference. drawing: The drawing id in archive. | Remove a drawing form a model. Only removes the link If you want to remove the drawing from the archive as well, use deletedrawing -command |
REMOVEITEM(child, mother, quantity) | child: Code to be removed. mother: The code of the parent item quantity: How many items are to be removed | Removes items from another item's structure. Requires Flow |
RENDER(filepath, h_resolution, v_resolution, type, radiosity, iteration, quality) | filepath: path to the output file h_resolution: horizontal resolution v_resolution: vertical resolution type: string as follows:
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radiosity: indirect lighting limit as percentage (10% is a good start) iteration: Iteration time of indirect lighting as seconds, 600 is a good value quality: quality of indirect lighting | Visualize active model to a file |
RUNPPROG(program) | program: The program path | Run a parametric language program |
SAVETOPDM(modelname, itemcode, savedrawings, archivefields, transfer_structure) | modelname: The archive model id of the active model. itemcode: Item code, ahich is created savedrawings: Save the drawings as well archivefields: Archive data as string in format FIELD=VALUE;FIELD2=VALUE... transfer_structure: 1 = Transfer structure as well, 0 = no structure | Check in the active model. Flow connection must be established. |
SETDOPLOT() | - | Plot 3D -model on screen. To be used in beginning of the task file. Causes slowness, only use when necessary |
SETFILESAVEOPTION(val) | val: How to pack the files when saving.
CODE
| Set how the saved model files are packed. |
SETFLAG(flag, value) | flag: the identifier of the flag to be set value: value of the flag
| Set certain parametres of the model or environment. Only for use after consulting Vertex. Do not use if you are even a bit uncertain of what you are doing. |
SETMETAPARAMS(part, parameter, type, on_off) | part: Reference to part or assembly parameter: Which parameter is manipulated
CODE
type: data type, “int” for others, “TF” for part_to_profile on_off: 1 = turn on, 0 = turn off | Use in the rarest of cases. |
SETOBJECTDATA(code, type, fields) | code: Code of item, whose data is manipulated type: type of object: “project” "item", "model" or "drawing" fields: list of attributes fields: FIELD=VALUE|FIELD2=VALUE... | Set object data to an item in FLOW |
SETSTRUCTUREDATA(main_item, structure_item, fields, overwrite) | main_item: The master item, whose structure is being manipulated structure_item: the actual structure item, which attibutes are being manipulated fields: list of attributes fields: FIELD=VALUE|FIELD2=VALUE... overwrite: 1, if you want to overwrite the existing attributes | Set structure data to an item in FLOW structure |
SLEEP(time) | time: Time to wait before automatically going on in milliseconds. | Pause the task execution for certain amount of time |
STARTPDF(settings) | settings: can be merely path to created pdf file, or list of pdf settings | Start a PDF file creation. Requires CREATEPDF later on. All drawings opened and saved betweeb STARTPDF and CREATEPDF will be in the PDF book. |
TRANSFER(document_id, ducument_name, filpath, archivefields) | document_id: The ID -code of the document. document_name: The decsription (name) filepath: file of the document to be transferred to Flow archivefields: Archive data in format FIELD=VALUE;FIELD2=VALUE... | Add any file to the Flow as a document. Flow connection must be established |
TRYOPEN(model, steps) | model: The archive name of the model to open steps: Number of lines to step over, if OPEN fails. If -1, step until the corresponding CLOSE -command is issued. | Opens a model from the archive, steps over certain amount of commands if open fails. this is to be used if yo uare uncertain wether the opened model exists. |
VIEWPOINT(vp_list) | vp_list can contain any number of these elements, in form:
CODE
x: X-coordinate of the eye point y: Y-coordinate of the eye point z: Z-coordinate of the eye point look_x: X-coordinate of the point to look at look_y: Y-coordinate of the point to look at look_z: Z-coordinate of the point to look at angle: view angle | Change the viewpoint on the model |
ZIP(folder, filter, path) | folder: Folder path , which contains the files to be packed filter: file filter to select the packed files path: zip-file path to be created | Packs files to compressed zip-package. |