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ACTIVATEPROJ(proj_id)

Create or activate a project.

proj_id: Name for project. Must conform to standard Vertex project naming rules.

ADD(part, filepath,rep_link)

Add a part to the assembly

part: reference to the part being added, May include the index (#100)

filepath: if the added part is not in archive, it can be read from file path, otherwise leave empty.

rep_link: determines 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 representation 2.

ADDADAPTIVE(model, subassy, repr, x, y, z, alfa, beta, gamma)

Add an adaptive component to the assembly. Used in conjuction with stopadaptivecomponent

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)

ADDGROUPBYREF(group, text, mode, X, Y, origin, angle)

Adds a 2D group to drawing. usesa agiven text as bases of placement.

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 choice (optional)

angle: Angle of the macro in degrees(counterclockwise) (optional)

ADDMEAS(view, direction, plane, location, pos, elem1. elem2, text, dimtype, height, sc, XplceElem, YplceElem, inchprec, prec)

OBSOLETE

Add a dimension to 3D -model, which can be shown also in the drawing. OBSOLETE, user ADD3DMEAS instead.

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

ADD3DMEAS(view, direction, plane, location, pos, elem1. elem2, text, dimtype, height, sc, XplceElem, YplceElem, inchprec, prec)

Add a dimension to 3D -model, which can be shown also in the drawing

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

ADDNEW(name, mode, ind)

Create an empty model to either an existing assembly or base window

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

ADDPNO

Add a part number to the model

ADDPNO3D

Locate 2D part numbers through 3d

OBSOLETE

ADDPROFILE(filepath,code,x1,y1,z1,x2,y2,z2, angle)

Adds a profile to the active assembly

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 angle counterclockwise

ADDSEARCHPART(part)

Adds a search part for ADDADAPTIVECOMPONENT

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.

ADDTABLEROW(Content,Sizes,AlignModes,CutModes)

Add a row to 2D text table. Used in conjunction with STARTTABLE and ENDTABLE.

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

ADDTEXT2D(type,dim_pt1, dim_pt2, dx, dy, text_angle, height, lorg, view_name, text, reflinepoints)

Adds text to 2d drawings

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)

ADDTEXTS(proj, MN, id, text_type, height, xt, yt)

Adds texts in macro points (added with ATTACHTEXTS) to a specified projection in a drawing

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

ASSYCHANGEREPRE(part, representation, remove_extra_parts)

Changes representation of a part/assy

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.

ATTACHDRAWING(drw)

Attach a drawing from the archive to a model

drw: Drawing name in archive. Drawing must be found in archive.

ATTACHTEXT(part, macroname, text, id)

Attach texts to a part. These texts can then be added to the drawing using ADDTEXTS.

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)

AUTOTESTINIT(mode)

Sets the user interface mode. To be used on as a background process with Flow

mode:

1 = command list and ui not visible

2 = UI visible

BREAKLINK(views)

Breaks the links between model and drawing for a certain view(s)

views: view names (optional)

CALCELEM(part, mode, filename, massunit, massaccuracy, locaccuracy)

Calculates the mass properties for a part or assembly

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

CHANGE(part1, part2, filepath, representation)

Changes parts or subassemblies in the active assembly

part1: Reference to the existing part

part2: Archive name of the new part

filepath: Complete path to an unarchived model to be added (optional, can be left empty)

representation: Representation in format Vnf, where n = representation number, f = F, if link, empty if local

CHANGEASSEMBLY(ref, target)

Move part or asseembly to another assembly in the model

ref: Part/assy to be put to antoher place in the structure

target: Reference to an existing assembly in the model

CHANGEPROFILE(part, filepath, dimensionset)

Change a profile section to another one

part: Reference to the profile part to be changed

filepath: Path from folder "proflibrary"

dimensionset: Dimensionset of the new part

CHANGESHEET(sheet_to_replace, replacing_sheet);

Replace drawing sheet to another

Drawing must be active

sheet_to_replace: Name of sheet to replace, e.g. “A4”

replacing_sheet: Either path to custom folder or the sheet id in Flow

CHECKMODELS(folder, save)

Check the model health. Open and save a folder or a project. Creates entries in VXTASK_DEBUG.

folder: Folder path or a project name to scan

save:

0: standard

1: all models are saved and backup from original will be made to user-directory

2: only active configuration is checked

4: warnings are considered errors

CLOSE(save)

Closes the active model window

save: is set to 1, model will not be saved when closing

CLOSEDRAWING(drawing)

Closes a drawing window

drawing: drawing number to be closed

CONNECTCONSTR(constraint_name, boundary_element, assemblyconstraint)

Connect constraints between assemble parts and adaptive component.

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

CONSTR(constraint, elem, alterntive1, alternative2, value, direction, closer)

Add an assembly constraint to the model

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)

CONSTR(elem1, elem2, x,y,z,alfa,beta,gamma)

Position two parts using macrolink-constraint

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

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)

Locate part using pre-defined constraint sets

ref1: Reference to part 1

ref2: Reference to part 2

setname1: Constraint set name for part 1

setname2: Constraint set name for part 2

COPYPASTE(0,part_name,posx, posy, posz,rotz,roty,rotx,kx,ky,kz)

Copies and pastes a part to another location

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

COPYVIEW(InstanceRef, DrawingName,ViewName, NewViewName, UpdateNew, X, Y, LocationType, scale)

Copies a projection from one drawing to another, while maintaining the update-capability

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"

CUTPROFILE(part, index, location_mode, pos, add_meas_points, add_insertion_points)

Cuts one long profile into separate given pieces

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

DBADDROW(db, fields)

Add a row to a database

db: Path to the database, e.g. “$DIR_SHARED/dbases/d_TIETOKANTA”

fields: Fields and their values, separated with a pipe. E.g. “field1=value1|field2=value2“;

DELATTRIB

DELPARTNUMBERS(ref)

Remove part number attribute (PNO) from a part or assembly

ref: reference to the parts, asseblies, of which part number it to be cleared

if empty, lear all part numbers in the assembly

DELVIEW(view)

Delete a projection from active drawing

view: projection name to be deleted

ENDTABLE(X,Y,ShowLines,Lorg,Height)

Create a 2D table on the drawing. Use in conjunction with STARTTABLE and ADDTABLEROW

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

EXECUTE(program, parameters, wait)

Execute an external application or a batch script

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

EXIT(save)

Exit Vertex

[obsolete] save.

EXPLODEVIEW(view)

Explode projection to lines

view: projection name to be exploded to lines

EXPORTPROJECT(proj, file)

Export project to vxz-file

proj: name of project to be exported
FileOrFolder is name of the file or folder to which export is done
If Project is empty, active project is exported

file: file to export to. If empty, <projectname>.vxz will be created

FILEOUT(path, mode, timestamp, line)

Writes a log file, or any other text file, line by 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

FILLADB()

Updates the attribute data rows from replacement array, where they are to be set with GLOBALVALUE -command.

-

GLOBALVALUE(key, value)

Set a value on the replacement array. Can be used to set text macros #KEY# to drawings etc.

key: nameof the replacementarray key

value: value to be set into the replacement array

LOCATE(part, xt, yt, zt, xr, yr, zr, xscale, yscale, zscale)

Similar way to mode parts as MOVE. Use MOVE instead of this

A different way to MOVE parts.

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)

MEASSET(part, meassetname)

Set the dimension set of a part

part: reference to the part.

meassetname: The measure set name.

MIRROR(removeoriginal, part, plane)

Mirrors the specified part or subassembly.

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

MMTOINCH(accuracy, type, remove_originals)

Convertes millimeter-based dimensions to inches in active drawing.

For detailed parameter values, see inch conversion tool in G4.

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.

MOVE(part, xt, yt, zt, xr, yr, zr, xscale, yscale, zscale)

Moves the specified part with translation and rotation. After moving the part, it will be fixed

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)

MOVEVIEW(viewname,viewx1,dim_pointx1,viewx2,dim_pointx2,viewy1,dim_pointy1,viewy2,dx,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.

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.

OPEN(model, mode)

Opens model

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

OPENDRAWING(part, drawing, mode, new_drawing)

Open a drawing from a local model, and update the drawing link to point to the new saved 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)

OPENFILE(filepath)

Opens an file from a file path

filepath: Full path to to any vxm, vxz or vxp, stp, sat, dwg… file. Opens all formats what can be opened with Vertex

PNOTODWG(part, view, text, dim_pt1, dim_pt2, dx1,dy1, dx2, dy2)

Adds a part number in a drawing

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

REMOVE(part)

Removes the specified part or subassembly from the assembly

part: Part or subassembly to remove

REMOVE2(part1, part2, … )

Removes all but the specified parts from the assembly

partn: Parts or subassemblies NOT to remove from the assembly

REMOVEFEATURES

Remove seelcted features from the active model

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

RESTOREPARAMS(type, param)

Restores pre-set parameters of geometry to original settings. Must be used with SETPARAMS

type: What type of object is restored (optional)

param: what type of parameter is reverted (optional)

SAVE(filename, ref, mode , lightmodel , ver )

Saves and exports the model.

Save packed *.vxz files

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 reference. If all. reference is “/” (optional)

mode: (optional)

save only this part = 0
leave the assembly as is, only save the part = +2
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 = +16
save 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

if saving a vxz -file, mode is

normal = 0
only main level = 1
main level and first subaseey level = 2

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)

SAVEDRAWING(drawing, path, setup, explode, <empty>, border_layer)

Saves an open drawing in several formats. Throws and error for incorrect file names.

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)

<empty>: This has been save version of the drawing file. It has been made obsolete in version 31. This is not needed, and should be left empty. A placeholder comma is needed, if border_layer -parameter is used.

border_layer: If given , you can define a layer by which the borders are updated. (optional)

SCALE(scale, slave_view, update)

Change scale of a projection

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.

SET2DCONSTRMGMT(onoff)

Set 2D constraint manager on or off

onoff: if set to 1, 2D constraint manager will be of for the rest of the task run.

SETATTRIB(part, fields, vxtype, mode)

Set attributes like BOM data for a specified part

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

SETCOLOR(part, color)

Changes the visualization material of the model

part: Reference to the part

color: Lightworks material name or Vertex palette number

SETMASSUNIT(value)

Sets the mass unit used with CALCELEM.

value: set mass and volume units to be used

0 = t  (tons)
1 = kg (kilograms)
2 = g (grams)
3 = mg (milligrams)
4 = lbs (pounds)

Corresponding volume units:

0 = m3  (cubic meters)
1 = dm3 (cubic decimeters)
2 = cm3 (cubic centimeters)
3 = mm3 (cubic millimeters)
4 = in3 (cubic inches)

SETMEAS(reference, value)

Changes a driving measure

meas: Reference to the measure. in format */assy/part.measname

value: Value of a measure.

SETNAME(part, newname)

Change the name of a local part

part: Reference to the local part

newname: New name

SETPARAMS(object, type, settings)

Sets parameters for selected objects. so far only Text is supported.

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=

SETSMDPARAM(part, bend_table)

Change the bending table or -formula of a part

part: Reference to a part tobe changed

bend_table: Bending table name or parametrica language program. Must be located in "bend" -folder

SETSTRPLATE(part, code)

Changes the thickness of a structured plate

part: Reference to the part.

code: The code, must be in the database

SKIPMASSCALC(mode)

Skip mass calculation to save time

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.

SOLVE(mode)

Solves the active assembly

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

SKIPMASSCALC(mode)

Skip time-consuming mass calculation

mode: 1, if mass calculation is skipped in tas run after this command, 0 if not.

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)

Translates the drawing with a translation database

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

UPDTEXTMACROS()

Updates text macros in the active drawing

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UPDVIEWS()

Updates 3D -projections in the active drawing

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VISIBILITY(part, visibility, represenstations)

Changes the visibility of a part in the active model

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").

VISIBILITYFAST(part, visibility, represenstations)

Changes the visibility of a part in the active model, really fast compared to the older version

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").

ADDITEM(child, mother, quantity)

Adds an item to another item's structure, requires Flow.

child: Type of the object to be created: "item", "customer", "project", ...

mother: Code of mother object. Must be unique

quantity: how many childs are added

BOOLEAN(parts_to_be_machined, machining_parts,action, offset, machining_parts)

Boolean operators

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

CLOSEDEBUGFILE()

Ends debug-redirect to custom file. After this debug logs goes back to ./VXTASK_DEBUG. Requires OPENDEBUGFILE -command to be used before.

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COLLECTFEATS(file)

Collect machining features form the model. Requires Hydraulic Block Design -option.

file: path to which the features are to be saved

COLLECT_PARTLIST(assy, file, formatfile , where, rollout, kompot_choise, repstr)

Collect parts list to text file, tranfer to product database or update the bom in sheet.

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

COLLISIONS()

Checks for any collisions in the model. Outputs to debug log file.

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COMPAREDRAWING(drawingname, leaveopen, tolerance)

Compares two drawings line by line

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"

COMPAREFILES(pic1, pic2)

Places two Vertex drawings on top of each other, and writes differences to VXTASK_DEBUG_file

pic1: File path to vxp file 1

pic2: File path to vxp file 2

CONNECT(obj_type1, obj_code1, obj_type2, obj_code2)

Connects two Flow-objects. Requires Flow.

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

CREATE(filename)

Creates a file to the file system. Like *nix “touch”.

Requires operator FILE_DIR

filename: name of file to be created

CREATEPDF()

Creates PDF book. Requires STARTPDF -command before.

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DELETEDRAWING(id)

Deletes drawing completely from the archive. Does not ask any confirmations.

id: archive number of the drawing to be deleted

DELETEMODEL(id)

Deletes model completely from the archive. Does not ask any confirmations.

id: archive number of the model to be deleted

DELETEPROJ(id)

Deletes project completely from the archive. Does not ask any confirmations.

id: archive number of the project to be deleted

DELITEM(itemcode, del_links, keep_item)

Deletes item from Flow. Requires Flow.

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

EDITPARTLINES(part, mode, viewname, layer, pen_width, sort, rsize, color)

Set 2D parameters of a part’s lines.

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

LOADSTUDIO(name)

Loads a predefined visualization studio

name: visualization studio name

MODELDATATOFILE(path, reference, skip_acis_check)

Save the model data to a text file

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

NOMESSAGES(no_messages)

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.

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.

OPENDEBUGFILE(file)

Redirect the output to a given file, unless this is used, it will be written to ./VXTASK_DEBUG. Remeber to close this with CLOSEDEBUGFILE

file: file path

PARTPLISTMODE(part, partplistmode)

Specifies how the parts are to be collected to the partslist

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

PAUSE()

If debugfeatures are set, this function adds a "breakpoint" to active modelling

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PDMPLISTTOXML(item,fields,file)

Item structure from Flow to XML

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

POINTCLOUDSCALE(part, scale)

Scales point could models

part: reference to the point cloud in the active model

scale: new scale either as numeric or string format

POINTCLOUDTHINOUT(part, dim)

Makes thinout to point clound parts

part: reference to the point cloud in the active model

dim: thinout dimension

REMOVEDRAWING(part, drawing)

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

part: The part or assembly reference.

drawing: The drawing id in archive.

REMOVEITEM(child, mother, quantity)

Removes items from another item's structure. Requires Flow

child: Code to be removed.

mother: The code of the parent item

quantity: How many items are to be removed

RENDER(filepath, h_resolution, v_resolution, type, radiosity, iteration, quality)

Visualize active model to a file

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

RUNPPROG(program)

Run a parametric language program

program: The program path

SAVETOPDM(modelname, itemcode, savedrawings, archivefields, transfer_structure)

Check in the active model. Flow connection must be established.

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

SETDOPLOT()

Plot 3D -model on screen. To be used in beginning of the task file. Causes slowness, only use when necessary

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SETFILESAVEOPTION(val)

Set how the saved model files are packed.

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

SETFLAG(flag, value)

Set certain parameters of the active model or environment. Only for use after consulting Vertex. Do not use if you are even a bit uncertain of what you are doing.

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

• TOASSYPARTLIST - part/assembly is collected to main assembly part list. Values ON, OFF

SETMETAPARAMS(part, parameter, type, on_off)

Use in the rarest of cases.

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

SETOBJECTDATA(type, code, fields)

Set object data to an item in FLOW

type: type of object: “project” "item", "model" or "drawing"

code: Code of item, whose data is manipulated

fields: list of attributes fields: FIELD=VALUE|FIELD2=VALUE...

SETSTRUCTUREDATA(main_item, structure_item, fields, overwrite)

Set structure data to an item in FLOW structure

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

SLEEP(time)

Pause the task execution for certain amount of time

time: Time to wait before automatically going on in milliseconds.

STARTPDF(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.

settings: can be merely path to created pdf file, or list of pdf settings

TRANSFER(document_id, ducument_name, filpath, archivefields)

Add any file to the Flow as a document. Flow connection must be established

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...

TRYOPEN(model, steps)

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.

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.

VIEWPOINT(vp_list)

Change the viewpoint on the model

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

ZIP(folder, filter, path)

Packs files to compressed zip-package.

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