Design automation commands

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

    assembly = 0
    assembly_to_existing_model = 1
    part = 2
    part_to_existing_model = 3

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
PARTNAME.R(R1).L(Z):1" explains that constraint named FLOORLEVEL will be connected to a face of part named 'FLOORLEVEL' which is found based on insertion point macro R1 location and it's Z-axis direction.

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 true delete constaraints and parts not included in representation.

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.

    center = 0
    lower_left = 1
    lower_right = 2
    upper_right = 3
    upper_left = 4
    relative_to_original = 5

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:

    distance_from_start = 1
    relative_pos_from_start = 2
    distance_from_end = -1
    relative_pos_from_end = -2

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:

    append = 0
    create_empty_and_append = 1
    delete_only = 2

timestamp:

    no_time_stamp = 0
    beginning_of_line = 1
    end_of_line = 2

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 1, remove the original part or assembly.

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 1 , remove original dimensions, otherwise mm and inch dimensions will appear on top of eachother, on different layers.

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

• name of model in the archive

• id of a model in Flow

• file path

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)

1 = do not update text macros
2 = draw macros fo ATTACHTEXT and ADDTEXT -commands
4 = open the drawings and save them, and close them at once
8 = do not update projections

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

    Depressions = 1
    Protrusions = 2
    BlendNetWorks = 4
    BlendSequenses = 8
    AllBlends = 12
    All = 15
    RemoveHistory = 1024

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

    Plane = 1
    CylinderOrCone = 2
    Sphere = 3
    Torus = 4
    IHaveNoIdea = 5
    Spline = 6
    ReverseCylinderOrCone = 12
    ReverseSphere = 13
    ReverseTorus = 14
    All = 60

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)

save only this part = 1
save all instances of the part = +2
leave the assembly as is, only save the part = +4
do not copy the drawing, but instead leave the drawing links intact to the old drawing = 4
remove drawing links= +8
use quicker saving for similar link models in the assembly = +16save with archive data (use original or GLOBAVALUES, if given) = +32
update drawings if model has been changed = +64
always update drawings = +128
save to Flow = +256

lightmodel: (optional)

normal = 0
shellmodel = 5
facetmodel = 6

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 1, update the drawing. Use only in the last scale -command.

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.
6 = part numbers added by ADDPNO3D ja PNOTODWG.
7 = dimensions added by ADDMEAS.

settings you can enter are:
LEVEL=,COLOR=,FONT=,DMODE=,UNDERLINE=,UNDERLINED=,COVER=,HIDE=,
BOX=,BOXED=,LORG=,LORG2=,HEIGHT=,ANGLE=,LINEWIDTH=,SLANT=,RWIDTH=,ESPACE=,RDISTA=,CLASSIFIER=,LABEL=

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.
This concerns only task in which command is given.

Skip mass calculation to save time

SOLVE(mode)

mode:

Public Enum solveoptions
    standard = 0
    machiningfeatures = 1
    external_references = 2
    links_to_local = 4
    check_acis_geometry = 8
    check_part_history = 16
    profile_part_history = 32
    solve_externals_afterwards = 64
    classic_dimensions = 128
    solve_classic_g4_externals = 256
    remove_machinings_before_solve = 512

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

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:

    subtract = 0
    add = 1
    intersect = 2
    intersect_with_tolerance = 2
    subtract_with_tool = 4

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 1, update the drawing bom.

to_database: if set to 1, bom is transferred to the database.

number_parts: if set to 1, number the unnumbered parts while transfering to database.

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:

    do_not_delete = 0
    delete_all_links = 1
    delete_drawings = 2
    delete_models = 4
    delete_drawing_formats = 8
    delete_model_formats = 16

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:

    Standard
    Stereo
    Panstripe
    Pancross

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.

0 = files will not be packed when saving
1 = files will be packed using the conventional method
2 = files will be packed using LZ4 -method (default)
-1 = use values defined in user/SETUP -file

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

• ALLCONSTRAINTSACTIVE - solve also the constraints which are disabled . Values ON, OFF

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

8 ="Explode to partlist", move the BOM data to upper level in the parts list while collecting
49 = "Alikokoonpanona ratkaistava" , solve subassembly if external refereces so require
0 = Change part to profile

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:

x=500,y=700,z=1000,look_x=0,look_y=0,look_z=0,angle=60

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.