hello,is it possibile to visit dimensions from a assembly drawing and get information about from which PART the dimensions is from? As far as I understand Creo it works as following:open assembly filecreate new drawing modelassembly-model (as one piece/element/whatever) is connected as drawing modelIf I try to visit dimensions I found "ProDrawingDimensionVisit" for reference (manually added) dimensions in the drawing and "ProDrawingSolidsVisit" for the dimensions from the drawing model. But both methods dont deliver any information from which part the dimension is driven from.E.g. just for assembly model (NOT drawing) it works just fine if I do:traverse through assembly-Model via "ProMdlDependenciesList"for each assembly model run again "ProMdlDependenciesList" (recursion)for each part model, call "ProSolidDimensionVisit"I cant use the same in drawing mode because I need some extra information (like in which view the dimension is) so I have to use "ProDrawingSolidsVisit". But:traverse through assembly-Model via "ProMdlDependenciesList"for each assembly model run again "ProMdlDependenciesList" (recursion)for each part model, call "ProDrawingSolidsVisit"is not working -> "PRO_TK_E_NOT_FOUND"maybe a function to add all assembly elements as drawing model?regardsThis thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

Hello,Go through below steps:ProDrawingSolidsCollect --> Will help you to identify all solids of drawing file. Find array size and loop through all solidsProSolidDimensionVisit ---> Visit the dimensions of solidProAnnotationIsShown ---> Use this API into Filter action of above visit. decide whether solid's dim is visible into drawing file or notBelow is the list of API to be called into visit action:ProDrawingDimensionViewGet --> Will get handle of view [Note: you will not get -4 here as you filtered in visit filter (ProAnnotationIsShown) that only shown annotations are visited.]ProDrawingViewNameGet ---> Will get name of the viewLet me know this works for you or not.RegardsKetan

L

lgüthle

1-Visitor

Solved

visit dimensions from (assembly) drawing

Forum|Forum|11 years ago
July 14, 2015
6 replies
2871 views

hello,

is it possibile to visit dimensions from a assembly drawing and get information about from which PART the dimensions is from? As far as I understand Creo it works as following:

open assembly file
create new drawing model
assembly-model (as one piece/element/whatever) is connected as drawing model

If I try to visit dimensions I found "ProDrawingDimensionVisit" for reference (manually added) dimensions in the drawing and "ProDrawingSolidsVisit" for the dimensions from the drawing model. But both methods dont deliver any information from which part the dimension is driven from.

E.g. just for assembly model (NOT drawing) it works just fine if I do:

traverse through assembly-Model via "ProMdlDependenciesList"
for each assembly model run again "ProMdlDependenciesList" (recursion)
for each part model, call "ProSolidDimensionVisit"

I cant use the same in drawing mode because I need some extra information (like in which view the dimension is) so I have to use "ProDrawingSolidsVisit". But:

traverse through assembly-Model via "ProMdlDependenciesList"
for each assembly model run again "ProMdlDependenciesList" (recursion)
for each part model, call "ProDrawingSolidsVisit"

is not working -> "PRO_TK_E_NOT_FOUND"

maybe a function to add all assembly elements as drawing model?

regards

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

2D Drawing

Best answer by Ketan_Lalcheta

Hello,

Go through below steps:

ProDrawingSolidsCollect --> Will help you to identify all solids of drawing file. Find array size and loop through all solids
ProSolidDimensionVisit ---> Visit the dimensions of solid
ProAnnotationIsShown ---> Use this API into Filter action of above visit. decide whether solid's dim is visible into drawing file or not
Below is the list of API to be called into visit action:
- ProDrawingDimensionViewGet --> Will get handle of view [Note: you will not get -4 here as you filtered in visit filter (ProAnnotationIsShown) that only shown annotations are visited.]
- ProDrawingViewNameGet ---> Will get name of the view

Let me know this works for you or not.

Regards

Ketan

K

Ketan_Lalcheta

2-Explorer

Hi,

I am able to find view details also for the dimension created in assembly. Only assumption I made is that dimension created into assembly must be visible into drawing file as well.

If still you are not able to get all details, I can look into your code snippet if you share it here.

Regards

Ketan

L

lgüthle

Author

1-Visitor

Ketan Lalcheta schrieb:

Only assumption I made is that dimension created into assembly must be visible into drawing file as well.

What do you mean with "must be visible into drawing file"?

here are my code snippets.

Derive Dimensions from 3D ASSEMBLY (working)

ProMdl mdl;

ProError status;

status = ProMdlCurrentGet(&mdl);

traverseModel(mdl);

traverseModel(ProMdl mdl){

     int i, n_mdl;

     ProModel *model_list;

     wchar_t name[80];

     wchar_t type[10];



     status = ProMdlDependenciesList (mdl, &model_list, &n_mdl);

     for( i=0; i<n_mdl; i++ ){

          wcscpy_s(name, 80, model_list[i].name);

          wcscpy_s(type, 10, model_list[i].type);

          if(wcsncmp(model_list[i].type, assembly,3) == 0 ){

               status = ProMdlRetrieve(model_list[i].name, PRO_MDL_ASSEMBLY, &mdlTemp);

               traverseCounter++;

               traverseModel(mdlTemp);

          }

          if(wcsncmp(model_list[i].type, part,3) == 0 ){

               if(traverseCounter==0){

                    getDimensions(mdl);

               } else {

                    status = ProMdlRetrieve(model_list[i].name, PRO_MDL_PART, &mdl);

                    getDimensions(mdl);

               }

     }

}

getDimensions(ProMdl mdl){

     ProBoolean refdim = PRO_B_FALSE;

     ProDimension *p_dims;

     status = ProArrayAlloc( 0, sizeof(ProDimension), 1, (ProArray*)&p_dims);

     status = ProSolidDimensionVisit( (ProSolid)mdl, refdim, (ProDimensionVisitAction)DimVisitAction, (ProDimensionFilterAction)NULL, (ProAppData)&p_dims);

     status = ProArrayFree( (ProArray*)&p_dims );

}

Attempt to derive dimensions with view details (not working):

ProMdl mdl;

ProError status;

status = ProMdlCurrentGet(&mdl);

traverseModel(mdl); <- the same as in 3D method but calling different getDimensions() method

getDimensionsDrawing(ProMdl mdl){

     ProDimension *p_dims;

     status = ProArrayAlloc( 0, sizeof(ProDimension), 1, (ProArray*)&p_dims);



     /* status for ProDrawingSolidsVisit = -4

        ProSolidDimVisitAction calls ProSolidDimensionVisit

     */

     status = ProDrawingSolidsVisit((ProDrawing)mdl, ProSolidDimVisitAction, NULL, (ProAppData)&p_dims); <- ERROR = -4

     status = ProArrayFree( (ProArray*)&p_dims );
}

Second attempt to derive dimensiosn with view details (not working as well):

ProMdl mdl;

ProSolid *solids;

status = ProArrayAlloc( 0, sizeof(ProDimension), 1, (ProArray*)&solids);

status = ProMdlCurrentGet(&mdl);

ProDrawingViewVisit((ProDrawing)mdl,ProTestViewVisitAction, NULL, (ProAppData)&solids);

ProArraySizeGet( solids, &numberSolids );

ProDimension *p_dims;

status = ProArrayAlloc( 0, sizeof(ProDimension), 1, (ProArray*)&p_dims);

for( i=0; i<numberSolids; i++ ){

     ProDrawing temp = (ProDrawing)&solids[i];

     status = ProMdlTypeGet((ProMdl)&solids[i], &mdltype);

     status = ProDrawingSolidsVisit(temp, ProSolidDimVisitAction, NULL, (ProAppData)&p_dims);

}

ProTestVewVisitAction(ProDrawing drawing, ProView view, ProError filterstatus, ProAppData data){

.... status = ProDrawingViewSolidGet (drawing, view, &solid);

...

     ProArrayObjectAdd((ProArray*)data, PRO_VALUE_UNUSED, 1, &solid);

}

Thanks for looking into my code!!

best regards

Luis

K

Ketan_Lalcheta

Answer

2-Explorer

Hello,

Go through below steps:

ProDrawingSolidsCollect --> Will help you to identify all solids of drawing file. Find array size and loop through all solids
ProSolidDimensionVisit ---> Visit the dimensions of solid
ProAnnotationIsShown ---> Use this API into Filter action of above visit. decide whether solid's dim is visible into drawing file or not
Below is the list of API to be called into visit action:
- ProDrawingDimensionViewGet --> Will get handle of view [Note: you will not get -4 here as you filtered in visit filter (ProAnnotationIsShown) that only shown annotations are visited.]
- ProDrawingViewNameGet ---> Will get name of the view

Let me know this works for you or not.

Regards

Ketan

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