your nested config structure scares me a little bit, but maybe it's for a good purpose.
If you use the "SM-FLAT-PATTERN" config for dxf you won't get bend lines. Save dxfs from the formed config if you want bend lines in dxf.
Here's the dxf method I wrote with tid-bits I picked up from others and SW help doc. Please excuse my literal strings. This is called from the PDM task add-in which provides whether or not to overwrite existing dxf and the method passes back a message that's stored in the task instance details.
In short it:
- to start out there's some logic to build the full dxf path, and if overwrite is set and file exists move it to the "OLD" folder. If the dxf fails I can put it back, if it succeeds then I leave it there.
- gets a list of all the configs, filters that list for any that contian "DXF" then adds "Default" at the end.
+ the "DXF" keyword is an arbitrary phrase that we selected for complicated parts that will not flatten without special edits. Also for laser cut parts that have chamfered holes (our laser cuts out the major diameter).
- next it loops through the list of configs and will use the first one that has a feature TYPE of FlatPattern and that has been working for our needs. Feature type "SheetMetal" might also work. However, I still go clean up the Flat Pattern feature sub-tree because of the random nature of users.
Here's the GetTypeName method I use:
https://help.solidworks.com/2019/Englis ... Redirect=1
- After doing my best to clean up the selected config I set some options that I learned about along the way, make sure the map file is set, etc. then try to save the dxf. That doesn't work try the next config in the list until either we have a dxf or run out of configs.
+ If a good dxf is created by SW, then I add a comment to the top of it at a bread crumb trail to myself. I should add the local version number of the file to that note...
Code: Select all
/*SaveDXF() needs the part (ModelDoc2 md2) to be active if its a Virtual Component in assembly.
* returns the path of the saved dxf, if file there and not over written then "" else null.
*/
private bool? SaveDXF(ModelDoc2 md2, string dxfFileName, bool overWrite, ref string msg)
{
string mapFilePath;
string archivePath = "";
bool? dxfCreated = null; //stores return value from ExportToDWG2() method.
string dxfSrcPath = md2.GetPathName();
PartDoc swPart;
swPart = (PartDoc)md2;
string dxfFullPath = System.IO.Path.Combine(getDXFpathByMtrl(ref swPart), dxfFileName);
dxfFullPath = Path.ChangeExtension(dxfFullPath, "DXF");
/* truth table for file exists and overwrite
* exists | overw | action
* -------------------------
* 0 | 0 | make new
* 0 | 1 | make new
* 1 | 0 | nothing, return msg
* 1 | 1 | move old then make new
*/
if (overWrite && File.Exists(dxfFullPath))
{
ExtensionsAndFunctions.MoveFileToOLD(dxfFullPath, out archivePath, ref msg);
}
if (!File.Exists(dxfFullPath))
{
//20201023-bnemec: trying to filter by flat feature in tree. (will be supressed)
//http://help.solidworks.com/2019/english/api/sldworksapi/Get_All_Sheet_Metal_Feature_Data_Example_CSharp.htm
//if (!md2.Visible)
// md2.Visible = true;
int actv8DocOptions = (int)swRebuildOnActivation_e.swDontRebuildActiveDoc;
swApp.ActivateDoc3(dxfSrcPath, false, actv8DocOptions, 0);
//to help performance per https://forum.solidworks.com/message/858283
md2.FeatureManager.EnableFeatureTree = false;
md2.FeatureManager.EnableFeatureTreeWindow = false;
//look for config with DXF in name else use Default
bool bShowConfig;
string[] configs = md2.GetConfigurationNames();
List<string> dxfConfigs = configs.Where(config => config.ToUpper().Contains("DXF")).ToList();
//since there may be more than one DXF config we'll use the first one that creates a dxf,
//so we'll add "Degault" config to the end of the list
dxfConfigs.Add("Default");
//20201015-bnemec: testing with configs that contain flat info.
//20201017 bnemec: commented the if because most legit sheet metal files don't get a flat config
//that config is only generated in the model if the flat view is added to a drawing.
/*20201029-bnemec:
brought the if back but instead of searching for FLAT I'm looking for the DXF keyword, this is for parts where
the we need a custom config for dxf creation to work, if a config with DXF in name is found we use that, else use
Default config
This is done: It looks like a better way to do this is look for sheet metal or flat FEATURE in the feature tree
rather than looking for flat config.
*/
foreach (var conf in dxfConfigs)
{
try
{
//activate (show) that config
bShowConfig = md2.ShowConfiguration2(conf);
//check to see if the config contains a sheet metal feature with flat pattern
bool flatPtrnFound = false;
Feature swFeat = (Feature)md2.FirstFeature();
while (swFeat != null)
{
/* ***TODO*** add logic here to supress non sheet metal stuff if needed, like flex, dome, dimple etc.
*/
string featName = swFeat.GetTypeName();
// Process top-level sheet metal features
if (featName == "FlatPattern")
{
flatPtrnFound = true;
//Make sure the flat feature is supressed, or else the dxf will not have bend lines.
//http://help.solidworks.com/2019/english/api/sldworksapi/solidworks.interop.sldworks~solidworks.interop.sldworks.ifeature~setsuppression2.html
swFeat.SetSuppression2((int)swFeatureSuppressionAction_e.swUnSuppressDependent, (int)swInConfigurationOpts_e.swThisConfiguration, null);
// unsupress flat pattern sub-features incase someone saved file with them supressed or else the dxf will show them formed.
Feature swSubFeat;
swSubFeat = (Feature)swFeat.GetFirstSubFeature();
while ((swSubFeat != null))
{
string subname = swSubFeat.GetTypeName();
string name = swSubFeat.Name;
if (swSubFeat.GetTypeName().Contains("UiBend"))
{
swSubFeat.SetSuppression2((int)swFeatureSuppressionAction_e.swUnSuppressFeature,
(int)swInConfigurationOpts_e.swThisConfiguration, null);
}
swSubFeat = (Feature)swSubFeat.GetNextSubFeature();
}
break; // get out of while loop and do not set swFeat to next feature.
}
swFeat = (Feature)swFeat.GetNextFeature();
}
if (flatPtrnFound)
{
object varAlignment;
double[] dataAlignment = new double[12];
string[] dataViews = new string[2];
//instead of setting x,y,z to 1.0, leave them all 0 and it does better job orienting flat.
dataAlignment[0] = 0.0;
dataAlignment[1] = 0.0;
dataAlignment[2] = 0.0;
dataAlignment[3] = 0.0;
dataAlignment[4] = 0.0;
dataAlignment[5] = 0.0;
dataAlignment[6] = 0.0;
dataAlignment[7] = 0.0;
dataAlignment[8] = 0.0;
dataAlignment[9] = 0.0;
dataAlignment[10] = 0.0;
dataAlignment[11] = 0.0;
varAlignment = dataAlignment;
/*
The bitmask for SheetMetalOptions is {12 11 10 9 8 7 6 5 4 3 2 1}, where each bit is either 0 or 1 as follows:
Bit #1: 1 to export flat-pattern geometry; 0 to not
Bit #2: 1 to include hidden edges; 0 to not
Bit #3: 1 to export bend lines; 0 to not
Bit #4: 1 to include sketches; 0 to not
Bit #5: 1 to merge coplanar faces; 0 to not
Bit #6: 1 to export library features; 0 to not
Bit #7: 1 to export forming tools; 0 to not
Bit #8: 0
Bit #9: 0
Bit #10: 0
Bit #11: 0
Bit #12: 1 to export bounding box; 0 to not
* flat-pattern geometry and bend lines, then Bits 1 and 3 are set, the bitmask is 0000101,
* and you need to set SheetMetalOptions = 2^0 + 2^2 = 1 + 4 = 5.
*/
int options = 5;
// we use a map file for the laser to get bend lines up. we've always used same settings for laser and thermwood
//didn't bother implementing map file for each right now. could be done though.
swApp.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swDxfMapping, true);
swApp.SetUserPreferenceToggle((int)swUserPreferenceToggle_e.swDXFDontShowMap, true);
mapFilePath = @"C:\Vault\CAD_Library\SW-DXF_map_LASER";
swApp.SetUserPreferenceStringListValue((int)swUserPreferenceStringListValue_e.swDxfMappingFiles, mapFilePath);
int index = swApp.GetUserPreferenceIntegerValue((int)swUserPreferenceIntegerValue_e.swDxfMappingFileIndex);
swApp.SetUserPreferenceIntegerValue((int)swUserPreferenceIntegerValue_e.swDxfMappingFileIndex, 0);
index = swApp.GetUserPreferenceIntegerValue((int)swUserPreferenceIntegerValue_e.swDxfMappingFileIndex);
//Export sheet metal to a single drawing file
//https://help.solidworks.com/2019/english/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IPartDoc~ExportToDWG2.html
dxfCreated = swPart.ExportToDWG2(dxfFullPath, dxfSrcPath, (int)swExportToDWG_e.swExportToDWG_ExportSheetMetal, true,
varAlignment, false, false, options, null);
if (dxfCreated == true && File.Exists(dxfFullPath))
{
msg += "Saved \"" + dxfFullPath + LB + "\" from model " + dxfSrcPath + LB +
" Configuration: " + conf + LB;
// I like adding a note block in the dxf with a bit of info that it was an autommated dxf.
string note = "999" + NL +
"THIS DXF FILE GENERATED FROM SOLIDWORKS BY PDM TASK ADD-IN" +
" FILE: " + dxfSrcPath +
" CONFIGURATION: " + conf +
" AT " + System.DateTime.Now.ToString() +
" USING MAP FILE: " + mapFilePath + NL;
ExtensionsAndFunctions.prepend(dxfFullPath, note);
//break out of the while (configs) loop once we have a good dxf.
break;
}
else
{
//tried and failed to save dxf from a config that had a FlatPattern feature, this would be an error.
//dxfCreated should be false here
msg += "Failed to save dxf from: " + dxfFullPath + " " + conf;
}
}
else
{
//no FlatPattern feature found in this configuration, move on.
//dxfCreated should = null here.
}
}
catch(Exception ex)
{
msg += "caught Exception in foreach(config): " + ex.Message + LB;
}
}
//at end of config foreach loop, if no dxf then need to put the old one back.
if (!File.Exists(dxfFullPath))
{
ExtensionsAndFunctions.MoveFileBack(archivePath, dxfFullPath);
}
}
else
{ // file exists and ! overwrite
msg += (("output file: " + dxfFullPath.Quotes() + " already exists and not set to overwrite.").Highlight() +
LB);
dxfFullPath = "";
}
return dxfCreated;
}
