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Best way to create a drawing template

wladimir_triller332
wladimir_triller332 Member Posts: 2 PRO
in Community Support

Hi everybody

Tried hardly to create a Drawing template with DIN 6771-1 style title block but wasn’t successful. Can anybody recommend the best way to get there ore a recourse where such a template can be downloaded? Would be very helpfull. I Added an image of how it is suppose to look like.

 

Thanks a lot.




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  • PeteYodis
    PeteYodis Moderator, Onshape Employees Posts: 594 image
    @wladimir_triller332  Here is the section of our help on custom templates that may be pertinent to you, as I suspect you may also be coming from using another CAD package (https://cad.onshape.com/help/#templates-custom.htm?Highlight=custom template):

    Using traditional CAD drawings as templates in Onshape

    Create an Onshape drawing template..

    In Onshape, create an empty drawing:

    1. At the template step, select Custom Template.
    2. Select Do not include the borders.
    3. Select Do not include the title block.
      1. Set size, standard, and other characteristics as needed.
    4. Click OK and close the open dialogs in the drawing.
    5. Import your exported traditional CAD drawing (in DWG/DXF format) into Onshape (through the  menu > Import).
    6. Open the empty drawing you created.
    7. Use Insert DWG/DXF  tool to insert the file just uploaded.

    8. To tweak the fonts, select the text and change the font to an internally supported font of your choice.

      1. To add Revision Table or Block functions:
        1. Generate a drawing using the newly uploaded DWG/DXF.
        2. Place a table where needed (for example, the upper right corner).
      2. To include a company logo in the drawing template:
        1. Upload the logo through the Insert Image command.
        2. Insert the newly uploaded image, properly place and size it in the drawing.
      3. Insert drawing fields as necessary in the appropriate areas of your drawing:
        1. Add a note to the drawing.
        2. Select the Insert field button.
        3. Use the Move to command on the View’s context menu (right-click) to add elements to: Title block, Border frame, and Border zones.

          Elements will be added to the corresponding layer: title block, border frame, or border zones.

    1. Export the drawing as a DWT.
    2. Upload the new DWT into an Onshape document (company-owned is preferred).
    3. Test the drawing template before using.
  • brian_brady
    brian_brady Member, Developers Posts: 505 EDU
    PeteYodis said:

    Using traditional CAD drawings as templates in Onshape

    Create an Onshape drawing template..

    In Onshape, create an empty drawing:

    1. At the template step, select Custom Template.
    2. Select Do not include the borders.
    3. Select Do not include the title block.
      1. Set size, standard, and other characteristics as needed.
    4. Click OK and close the open dialogs in the drawing.
    5. Import your exported traditional CAD drawing (in DWG/DXF format) into Onshape (through the  menu > Import).
    @PeteYodis

    Ideally this could be done without a second CAD program. I would prefer to stay in just one, and that would be Onshape. 
  • PeteYodis
    PeteYodis Moderator, Onshape Employees Posts: 594 image
    edited July 2017
    @brian_brady These instructions would be for users that are migrating from another CAD package.  There is no need to re-invent the wheel inside Onshape.  This process is quick.  It marries the look of a drawing from another CAD package with all the proper behaviors of an Onshape environment.

    If you are starting purely from scratch, want to stay all within one Onshape environment, and you want some completely custom template; you could certainly use our powerful sketcher and sketch away, then export to DXF/DWG and use the method above.  You wouldn't have to leave the Onshape environment at all.
  • brian_brady
    brian_brady Member, Developers Posts: 505 EDU
    Doh. I hadn't thought of that. What about textual tags though? 
  • Jake_Rosenfeld
    Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646 image
    edited July 2017
    Hi Brian!

    The full text of the help article Pete is referencing mentions how to add title blocks, borders, etc:

    https://cad.onshape.com/help/#templates-custom.htm

    (Basically it boils down to adding a note and attaching it to the appropriate layer with right click > move to)
    Jake Rosenfeld - Modeling Team
  • brian_brady
    brian_brady Member, Developers Posts: 505 EDU
    Jake_Rosenfeld said:
    Hi Brian!

    The full text of the help article Pete is referencing mentions how to add title blocks, borders, etc:

    https://cad.onshape.com/help/#templates-custom.htm

    (Basically it boils down to adding a note and attaching it to the appropriate layer with right click > move to)
    @Jake_Rosenfeld

    I must be dense this morning, because I cannot find anything in the link you gave that describes adding text to a template using Onshape tools. Ideally I would like to completely remain in Onshape to perform all CAD work, including creating and saving custom templates without having to add text to the template everytime I make a new drawing. I think a video or other tutorial is in order. 
  • Jake_Rosenfeld
    Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646 image
    Hi Brian,

    There was recently a webinar about drawings in general:
    https://www.onshape.com/videos/custom-properties-drawings-and-drawing-templates-webinar-03-21-17
    There is information about templates at 16:00 and in the summary at the end.

    I'm not really sure of your workflow, but you can create a template with text in it in the following way:
    1. Create a drawing in onshape that will serve as your template.  This can be done in many ways. Some ways already mentioned in this thread were: importing a drawing from an external CAD system, or using the sketcher to make a DXF and then opening that DXF as a drawing.  Some ways that weren't mentioned in this thread: opening a template that already exists in the system and editing it, or creating a blank drawing and using the 'line' tool to set up the template.
    2. Add text to your drawing as you normally would (using the 'note' tool).
    3. Attach these note to the appropriate layer of the drawing by right clicking and using 'move to'
    4. Export your drawing as a '.dwt' ( https://cad.onshape.com/help/Content/templates-custom.htm#Exportin )
    5. Reimport that saved '.dwt' into some Onshape document (The webinar recommends importing all your custom drawings templates into a document called 'drawings templates', but you can organize this any way you want).
    You will never have to touch another CAD system when you use this workflow.  You will have to download the .dwt to your file system and reupload it to Onshape.  This is a limitation we are aware of and a fix is coming soon to make this workflow a bit easier.
    Jake Rosenfeld - Modeling Team
  • brian_brady
    brian_brady Member, Developers Posts: 505 EDU
    @Jake_Rosenfeld In step 1 you say "create a drawing in Onshape". Does this actually mean create a sketch in a Part Studio and export it or use the very limited tool set in a Drawing to create the template?
  • Jake_Rosenfeld
    Jake_Rosenfeld Moderator, Onshape Employees, Developers Posts: 1,646 image
    edited July 2017
    Brian,

    When I say "create a drawing in Onshape" I mean that you will need to have an Onshape Drawing tab with a Drawing that you want to turn into a template.  You can accomplish this in many ways, but it seems like you would like to use the Onshape sketch tools. Here are some steps for that:

    1. Make a sketch that you would like to turn into a Drawing
    2. Right click on the sketch in the feature tree and select "Export as DXF/DWG"
    3. Export the sketch (you will not need to change the default settings in this dialog)
    4. Click the "+" button in the bottom corner of the Part Studio
    5. Click "Import..."
    6. Find the file you just exported in your "Downloads" folder (or wherever your downloads go) and import it. This will add two tabs to your Document, a "blob" tab holding the file you just uploaded, and a Drawing tab containing the sketch.  You can ignore both of these tabs.
    7. Click the "+" in the bottom left corner
    8. Click the "Create Drawing..." button
    9. Go to "Custom template"
    10. Decide what standards you would like to use and what you want your borders to look like
    11. Make sure you select "Do not include" on the "title block" section (I assume the whole point of what you want to do is create your own title bock?)
    12. Click "OK"
    13. Click the Insert DXF button in the top right corner of the drawing
    14. Select the sketch you exported/reimported earlier
    15. Edit/resize/etc until you are happy with how the Drawing template looks
    16. Add text and export to ".dwt" with the above directions
    I hope this has been more helpful? If not, it's hard to give the right instructions without knowing what you are trying to accomplish.  Are you trying to create a title block entirely from scratch using our sketch tools? Do you like the look of a template that already exists and want to edit it slightly and add your own persistent text tags?  The high level overview is:
    1. Create an Onshape Drawing tab 
    2. Tailor it to exactly how you would like it to look (this could include importing sketches/DXFs/DWGs or using the built-in drawings tools, or adding notes, etc)
    3. Export it as .dwt
    4. Import it back into Onshape.
    Jake Rosenfeld - Modeling Team
  • brian_brady
    brian_brady Member, Developers Posts: 505 EDU
    @Jake_Rosenfeld

    I don't have a specific template look at this point. I was merely playing the devil's advocate. In reading this thread I was hearing "use another CAD program to make a custom title block for our CAD program because our program does not have robust enough drawing tools in Drawing mode to do the job." Maybe I was reading that into it myself. If I were a design department, I would question the need to buy a different CAD program to do what should be easily accomplished in the primary CAD program I am paying for.

    I am pulling for Onshape to be the only CAD system for lots of people in the future. It just needs more polish to have all of the tools necessary, especially in Drawings. 
  • wladimir_triller332
    wladimir_triller332 Member Posts: 2 PRO
    @ Pete

    Hi Pete, thanks for the manual. It workt very fine. Thanks
  • Nickolas_Lockard
    Nickolas_Lockard OS Professional Posts: 36 ✭✭
    Ugh, Drawings keeps reverting to really weird paper size, messed up title blocks, and screwy measurements. I think it's totally broken. :(

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