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To reuse an AutoCAD block in future Inventor drawings, import it into an Inventor DWG template, then save the template. In Inventor, choose Annotate → Symbols → Import AutoCAD Block, select the source DWG and block definition, set its scale and rotation, and insert it. The block will be stored under Drawing Resources → AutoCAD Blocks for new drawings created from that template. If your template is an IDW, use an Inventor Sketch Symbol instead: native AutoCAD block import is a DWG workflow.
First check whether your template is DWG or IDW
The file extension determines the right method. Inventor’s Import AutoCAD Block command imports AutoCAD block definitions into DWG drawings. It does not add native AutoCAD blocks to an IDW template. In an IDW workflow, make a reusable Inventor Sketch Symbol instead.
Inventor can place and adjust imported AutoCAD block instances, but it cannot create or edit the underlying AutoCAD block definition. If the definition needs changes, edit the source in AutoCAD and import the revised block into the Inventor DWG template.
Prepare the source DWG
The source file must contain a real block definition. Loose lines, text, or exploded geometry will not appear as a selectable block in the import dialog.
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- Open the source DWG in AutoCAD and run
INSERT. Check whether the required block is listed. - If it is not listed, select the intended objects and create a block with
BLOCK. Give it a clear name and a useful base point for placement. - Make sure required variable text is defined as block attributes, rather than ordinary text. Save the DWG.
- Check the source drawing’s units and the block’s intended scale. Note a known dimension so you can verify its size after import.
When an AutoCAD DWG is used as an Inventor drawing template, most loose AutoCAD graphical data is removed; block definitions and instances are retained. If graphics need to persist as reusable content, make them a block before bringing them into the Inventor template. See Autodesk’s drawing template guidance.
Import the block into an Inventor DWG template
- Open the template. Open the Inventor drawing template you want to update. If you are starting from a new drawing, choose the appropriate DWG-based template. Back up the template before changing it.
- Start the command. Use Annotate tab → Symbols panel → Import AutoCAD Block. You can also expand Drawing Resources in the browser, right-click AutoCAD Blocks, and choose Import AutoCAD Block. Menu placement can vary slightly by Inventor release or customized ribbon.
- Select the source file and definition. Browse to the source
.dwg, select it, then choose the required block from the definitions listed in the dialog. - Set scale and rotation. Enter the scale factor and insertion rotation. A factor below 1 reduces size; a factor above 1 enlarges it. Do not assume Inventor will correct every source/target unit mismatch automatically. Check the units and compare a known dimension after placement.
- Insert the instance. Click Insert, then click on the sheet to place the block. If it has attributes, Inventor opens the Edit Attribute dialog; enter the values and click OK.
- Finish or add more. Click again to place additional instances of that imported block. Right-click and choose Done to finish, or Restart to return to block selection and import another definition.
- Save the template. Use Save Copy As if you want to preserve the original, and save the updated file as an Inventor drawing
.dwgin the template location used by your active project.
Autodesk documents the ribbon and browser import paths and the scale/rotation controls in its Import AutoCAD Block reference. The block resource is listed under Drawing Resources → AutoCAD Blocks; see the Inventor AutoCAD Blocks help.
Verify that reuse works
Do not stop at saving the template. Create a new drawing from the updated template and expand Drawing Resources → AutoCAD Blocks. Confirm that the definition is present, insert a test instance, and check its size, orientation, and attribute values. A template update makes the resource available to drawings created from that template; it does not automatically add the block to drawings that already exist.
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In a drawing, the block definition is the reusable resource under Drawing Resources; a block instance is one placement on a sheet. Attribute values belong to an instance, so they can differ between placements without changing the definition. Select an instance to move, rotate, or scale it. Right-click and choose Edit Attributes to change its attribute values. The Static property controls whether grip points appear when the instance is selected. Appearance can depend on whether source objects use ByLayer, ByBlock, or explicit color, linetype, and lineweight settings.
If the template is IDW: use a Sketch Symbol
For an IDW template, create an Inventor Sketch Symbol from the AutoCAD content. Sketch Symbols can include 2D geometry, text, iProperties, prompted entries, and imported bitmap images, and a symbol saved in a template is available in drawings created from it. Autodesk’s Sketch Symbol documentation describes translating AutoCAD content into a symbol.
- Open or create the Inventor drawing and start a new Sketch Symbol definition.
- Import or translate the required AutoCAD geometry into the symbol. Define a sensible insertion point and any connection points.
- Add prompted text or iProperties if you need users to supply values when placing the symbol.
- Save the symbol in the drawing, then save the drawing as the template. Test it by creating a new drawing and placing the symbol.
This is not a lossless conversion of an intelligent AutoCAD block. Nested blocks are flattened into one symbol, and translated entities become sketch lines and arcs. AutoCAD attribute and dynamic-block intelligence does not carry over as native block behavior. For a larger Inventor symbol collection shared across users, Autodesk also supports external IDW or DWG Sketch Symbol libraries; the documented default library location is under C:UsersPublicDocumentsAutodeskInventor [release number]Design DataSymbol Library, but local configuration and release can change the path.
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Choose the right workflow
| What you need | Use |
|---|---|
| Retain an AutoCAD block definition and use its attributes in an Inventor DWG drawing | Import AutoCAD Block into a DWG template |
| Reuse a symbol in an IDW template, or use Inventor prompted entries or iProperties | Inventor Sketch Symbol |
| Bring geometry into a sketch for editing or constraining, rather than preserve a reusable block definition | Insert/translate DWG or DXF into an Inventor sketch |
| Make a large Inventor symbol collection available to multiple users | Controlled template distribution or a shared Sketch Symbol library |
Importing a DWG into a sketch is a different workflow from importing a block into Drawing Resources. In an active 2D sketch, use Insert panel → ACAD to translate selected DWG or DXF geometry. That is useful for editable sketch geometry, but is not the cleanest route when the goal is to preserve a reusable AutoCAD block with attributes. See Autodesk’s DWG/DXF sketch import guidance.
Troubleshooting
No blocks appear in the Import AutoCAD Block dialog
The DWG may contain loose geometry, an exploded block, or the wrong source file. Open it in AutoCAD, run INSERT, and check for the definition. If it is absent, recreate it with BLOCK, save the DWG, and retry. Autodesk recommends this check in its block-import troubleshooting article.
The block is the wrong size
Check source and target units, the block’s authoring scale and base point, and the scale entered in the import dialog. Compare a known dimension, then apply a deliberate scale factor or standardize the source block’s units. Also check whether the content was authored for paper space but is being used at a different drawing scale.
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Attributes are missing or do not prompt
Confirm in AutoCAD that the source block contains attribute definitions, not just text. Use the Import AutoCAD Block workflow into a DWG drawing, then edit values on the placed instance. A Sketch Symbol conversion does not preserve native AutoCAD attribute behavior.
A dynamic block has the wrong configuration
Inventor inserts a dynamic block using the default configuration from its definition; it is not a full environment for editing AutoCAD dynamic parameters or visibility states. If multiple configurations are needed, make separate static block definitions for Inventor, keep dynamic editing in AutoCAD, or rebuild annotation variability as a Sketch Symbol with prompted entries where appropriate.
The definition cannot be edited in Inventor
That is expected: Inventor can import and place AutoCAD blocks but cannot create or edit their definitions. Modify the source in AutoCAD, save it, and import the revised definition into the template.
The resource is missing from an existing drawing
Template resources are inherited by new drawings created from that template, not retroactively applied to old files. Import the block into the existing drawing, copy the drawing resource, or use Inventor’s Drawing Resource Transfer Wizard to transfer resources between files. After copying, verify the result in the destination drawing.
Prompted entries change or fail after resource transfer
For Sketch Symbols, prompted entries may not transfer correctly if definitions differ between source and destination. Check prompt order and names, property references, formatting, and symbol definition names; test the transferred symbol before distributing the destination template.
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