the script language"COMP_FEAT_RELATION"

[伟曹]

hello:

may i have a question about "COMP_FEAT_RELATION"

I study and look all tab files and find three places about "COMP_FEAT_RELATION"

FIRST: \afx\parts\equipment\bosch\schutzzaunsystemeinhaengewinkel_set.tab

SEARCH_COMP_OWNER_REF RAHMENTEIL CSYS ACS0 PLAZIERUNGSKOORDINATENSYSTEM

…

ASSEMBLE THIS_MEASURECOPY

WINKEL_MEASURE ANGLE1 ANGLE2

CSYS PLAZIERUNGSKOORDINATENSYSTEM REF_CSYS

COMP_FEAT_RELATION RAHMEN_H PLAZIERUNGSKOORDINATENSYSTEM DISTANCE2

COMP_FEAT_RELATION RAHMEN_B PLAZIERUNGSKOORDINATENSYSTEM DISTANCE1

END_ASSEMBLE

…

SECOND:\afx\parts\equipment\steel_construction_mm\beam_endcaps\endcap_rect.tab

ASSEMBLE THIS

CSYS PROFILE_END_CSYS CAP_CSYS

COMP_FEAT_RELATION W PROFILE_END B

COMP_FEAT_RELATION H PROFILE_END H

END_ASSEMBLE

THIRD:\afx\parts\equipment\steel_construction_mm\ladders\ladder_cage_1.tab

SEARCH_COMP_OWNER_REF LADDER_PART PLANE LADDER_PLANE ATTACH_PLANE

SEARCH_COMP_OWNER_REF LADDER_PART PLANE CAVE_TOP TOP_PLANE

SEARCH_COMP_OWNER_REF LADDER_PART PLANE A_XZ BOTTOM_PLANE

SEARCH_COMP_OWNER_REF LADDER_PART PLANE A_YZ CENTER_PLANE

…

ASSEMBLE THIS_MEASURECOPY

H_MEASURE DISTANCE

ALIGN BOTTOM_PLANE A_XZ

ALIGN ATTACH_PLANE A_XY

ALIGN CENTER_PLANE A_YZ

COMP_FEAT_RELATION W ATTACH_PLANE W_OUT

END_ASSEMBLE

…

I don't understand this script language(COMP_FEAT_RELATION and SEARCH_COMP_OWNER_REF ) ,can you explain these for me?

for example:    SEARCH_MDL_REF Model Filter Name Variable

Model = "Model name" | THIS | THIS_# | ASSEMBLY

--> Model name = can be defined through USER_SELECT by entering the chosen variable

--> # = Component ID (Only in assemblies)

Filter = SURFACE | EDGE | PLANE | AXIS | POINT | CSYS | QUILT

NAME = "Feature name" (Name of the feature, e.g. DTM1)

who can help me!!

thanks!!!

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[SamuelBrantner]

Hi 伟 曹‌,

here is the definition of the two commands:

Create Relations

The following command will create a component relation in the assembly, where the

component will be assembled into.

COMP_FEAT_RELATION DIM_COMPONENT REFERENCE_PART DIM_REFERENCE_PART

DIM_COMPONENT = Dimension of the model to assemble

REFERENCE_PART = Part to look in for an dimension. can be defined through USER_SELECT

DIM_REFERENCE_PART = Dimension of the reference part

Example:

COMP_FEAT_RELATION W PROFILE_END B

Will create a component relation in the assembly.  In this case it will be W:20 =

B:6.

This means, that the dimension W of the component to assemble will be equal to B

of the component you selected (PROFILE_END).

Search in owner model

The following command is used, to search for a certain reference in the owner model

and store its information in a variable.

SEARCH_COMP_OWNER_REF Model Filter Name Variable

Model = "Model name" | THIS | THIS_# | ASSEMBLY

--> Model name = can be defined through USER_SELECT by entering the chosen variable

--> # = Component ID (Only in assemblies)

Filter = SURFACE | EDGE | PLANE | AXIS | POINT | CSYS | QUILT

NAME = "Feature name" (Name of the feature, e.g. DTM1)

Example:

SEARCH_COMP_OWNER_REF LADDER_PART PLANE CAVE_TOP TOP_PLANE

Searches in the owner model defined through LADDER_PART (e.g. Ladder.asm) for a plane called CAVE_TOP

and stores its result in the variable TOP_PLANE.

Greetings Sam