Let me drop a couple of words on getting flat patters from imported components. I've seen a lot of imported parts lately created in other cad packages (Catia in this case) with punches that Inventor has problem creating flat pattern for.
The secret here is to use delete face with heal on and delete the inside of the punch first and only afterwards the outside faces of the punch in a separate delete operation. You can select inside faces of all punches for your first delete face operation.
If your vendor exported an assembly with one part, Inventor will imported it as multi-body part with one body and it will complain that it can't be converted to sheet metal.
In this case you can export it again to a neutral file format and import that back or you can use derive to get it all as one body.
When you try and convert to sheet metal you will see that inventor complains about having multiple bodies so we need to derive it into a single body.
1. Open a new part.
2. Go to 3d model / create/ derive and browse to our file : 141017 Sheet metal imports.ipt
3. In the derived part dialog, expand solid bodies, and unmark Body.1 (you only need to have Body.13)
4. On the derived style select single solid body and click ok.
Even though we have only one body it seems that the round inserts at the end of the arms are modeled in so we need to remove them to a constant thickness part.
5. Extrude-cut the sheet metal nuts (round inserts)
6. Select the inside faces of the punches, one at a time or all at once. Start the delete face operation and after marking heal option click ok. You should have something as in the images bellow.
7. Repeat the operation again for the outside faces of the punches. The end result should be like this:
8. Verify the thickness and change it accordingly in the sheet metal options.
9. Use flat pattern. You might need to select one face (inside face) before flat patterning if it doesn't unfold. You might also need to delete the existing flat pattern if any to get it to compute.
Today I'll show you my way of showing part info on dxf exported drawings. Every once in a while we do dxf profiles of flat pattern sheet metal parts and we need to add more info to each export. We don't always have time to do a drawing for each part but we add views of flat pattern parts on the main assembly layout (or in separate sheets) so we need the extra info on the views for the manufacturer.
We normally have: Part number, Material, Quantity, and Thickness as a note linked to each flat pattern view.
Here's how we do it:
1. First you need to expose the Thickness parameter of the model so go in functions (part environment) and mark "Export" box on Thickness. I would suggest you do this on the sheet metal template and maybe part template as well (in case you use the convert to sheet metal option).
This will add the thickness in custom iproperties of the part.
2. Create a drawing and add a view of a sheet metal part.
3. Add a custom symbol and in the sketch start a text with the following values:
Part Number: <PART NUMBER> link this to the model properties.
Material: <MATERIAL> link this to the model properties.
Finish the symbol creation for now.
4. Add custom part iproperties PJ_QTY :
4.(a) manually in the part properties
4.(b) In the BOM of the assembly. Open the BOM inside the main assembly (main project assembly) and go to parts only (you might need to enable it first). Click on add custom iproperties, type Thickness and type PJ_QTY (or whatever your want to call the part quantity). Add "Item Quantity" and have it next to PJ_QTY. Select the values on the Item Quantity and drag the lower corner of the last cell towards the PJ_QTY row just like in Excel. The PJ_QTY part properties gets created on all parts with the value from Item Quantity on it.
5. Go back to the drawing and place your symbol on an edge of your sheet metal part just like you would do with a balloon.
6. Edit the symbol, and the text in it. Because we linked it to a part with custom iproperties they are available to be referenced. Let's add the following text:
Quantity: <PJ_QTY> link this to the custom properties of the model.
Thickness: <THICKNESS> link it to the custom properties of the model as well.
7. Finish the symbol editing.
Now you can copy/insert it on any view, on any drawing before dxf export.
I would suggest that you copy it to the drawing template ready to drop in when needed.
Notes:
If you want to add Thickness to standard.ipt template you would be better to open it, convert it to sheet metal and back to normal. The parameters are part of it now and you can mark export on Thickness.
And the video:
In AIP 2015 that I am using now it exports fine but if the dxf export shows up <PART NUMBER> instead of the actual value you need to tweak your export options to convert Drawing Symbols to Blocks.
In the Save As dialog click Options, then click Next in the DXF Export Options and in the Export Destination window click on Mapping Options. In the General tab click Convert Drawing Symbols to Blocks. You can save the configuration for later reuse if you want.
If you need to explode the block in Autocad head over to Express Tools (this needs to be marked at installation it doesn't' come by default) and then use Explode Attributes rather than using the explode command.
In 2015 no matter of the settings in the save as options or the explode method it's working but in older versions I remember needing to take this steps.
I have just spent the last couple of
days playing with iLogic. I am doing a tank template that I will
present in the next couple of posts and it's all been done with
iLogic and iFeatures.
Meanwhile I decided to present you a
couple of iLogic routines and programs I am using. I have collected a
couple and hope you will find them useful.
I don't have any programming
experience, so all codes have been downloaded off the internet, tried
and tested.
The main ones that I use are Export
to PDF, DWF, and DXF. The reason I use ilogic is to automatically add
revision to the filename. You can also chose export folder so one
more thing out of the way.
I also use iLogic to force update
iProperties of the drawing from the model. I have a code to set the
scale of the model in the drawing and one to add virtual parts to the
assembly from a text document. (Curtis Waguespack's code). He also
gives a code to force turning all features off down level on all
components (huge time saver)
Create a folder for your iLogic codes,
recommend to use a map network drive location so they are available
for all users in your company.
Open a file and go to Manage \ iLogic
\ iLogic Browser , switch to External Rules tab. Right click and add
external rule. Add your rules, in my case UpdateProps (force update
of properties), SavePDF, SaveDXF, SaveDWF.
Switch to Global Forms and Add Form.
If you have a common Design Data folder on the network then this Form
will be available to all users ;) . Drag your rules on the right and
change the name of the buttons and of the form if needed.
I know you can add buttons on the
ribbon and quick access bar but you need to configure it with every
new Inventor release so I prefer to have a global form instead.
At times I need to do a batch of files
so I use Code Injector, a small utility that will do that for you. We
once had around 900 drawings to export to dxf and pdf so we just left
the injector run overnight. Here is the post and description.
http://beinginventive.typepad.com/being-inventive/2012/02/injecting-ilogic-code-and-ilogic-event-triggers-automatically.html
Virtual Components Issue: You have a number of standard Virtual parts that you find yourself adding over and over. You'd like to have the ability to add them based on a predefined list. Check his blog here for the code.
I use this to add various stuff like: oil for gearboxes and hydraulic units, paint and primer, chemical for anchor bolts, grout, etc.
Work Features Issue: You have other members of your design team that do not remember to turn off work features at the part level or sub-assembly level when they are done working with those files. As a result file previews and view representations get messed up. You'd like to have a quick way to toggle all of the work features off. Can this be done with iLogic? Check his blog here for the code.
Update copied properties. Issue: You have a lot of drawings that need update copied iproperties of the model (updates copied iproperties of the model in the drawing). Solution: Use the code to force the drawing to update copied properties from the model. Can be used with Code Injector to do a batch of drawings at a time. File to be used: UpdateProps.iLogicVb
Save PDF Issue: You have to export one or many drawings at a time to pdf. Solution: Use the code to export current drawing to pdf. It creates (if didn't exist) a folder called DXF on same path as drawing (needs saving first) in which a pdfwith the filename being "Drawing_filename + Drawing_description + Revision". Can be used with Code Injector to do a batch of drawings at a time. Make SURE that the drawing is saved otherwise the path of the folder and pdf will be on root drive. Save DXF Issue: You have to export one or many drawings at a time to dxf. Solution: Use the code to export current drawing to dxf. It creates (if didn't exist) a folder called DXF on same path as drawing (needs saving first) in which a dxf with the filename being "Drawing_filename + Drawing_description + Revision". Can be used with Code Injector to do a batch of drawings at a time. Make SURE that the drawing is saved otherwise the path of the folder and dxf will be on root drive.
Scale of first view in titleblock
In order to have the scale show up and update automatically in the titleblock, do the following. Edit your title block definition and add a Text item with the type Prompted Entry This text should contain <Scale>
After you add this, Inventor will prompt you for a Scale value whenever you add the title block to a sheet. The same happens when you add a new sheet with the title block to the drawing or when you start a new drawing using a template where you have applied this solution. When it prompts you, just leave the value blank
Then add the rule in text bellow to the drawing File to be used: Prompted_Scale.txt Add the rule to the trigger “Before Save Document”
After that, on every sheet in the drawing, you will get the scale value from the first view on that sheet in the title block when you save the file.
What
rules do you use? Please let me kow what's your favorite?
