The work with curves is terrible..

[dxmv]

Hello. I keep running into this problem! Inventor is very slow in processing vector and curves and splines!!! Editing elements with a lot of curves takes weeks... Combining curves into blocks does not do anything, because in the process of work all the same have to edit a lot of curves. How do I make working with curves in Inventor as pleasant as in Rhinoceros?

[CGBenner]

@dxmv 

Wow, that is a lot of points for a single sketch.  Curious what you're making (if you can tell us).

Also, can you share a little about the hardware you're doing this on?

[swalton]

Are you able to re-model the artwork from scratch to approximate the detail in the curve file?

The Inventor sketcher likes fully defined geometry on the scale of 10-100 entities, not 1000s of entities.   It is usually better to build the final 3d shape from many simple sketches, extrusions, and surfaces, not from a single very complex sketch.

How about exporting a water-tight surface or solid from Rhino and use that to modify an Inventor part?  This may be a process where using the surfacing tools from another package will get a faster result than a pure Inventor model.

[johnsonshiue]

Hi! I don't think Inventor is the right tool for this design. It is because each piece of geometry in Inventor has to carry design intent and it has to be measurable.

An art work like this does not fit the above criteria, which is why it is difficult. I suggest you look into Fusion 360. It offers more flexible modeling paradigms (Direct Modeling, Mesh Design, Freeform TSpline, and Generative Design).

Many thanks!

[JDMather]

---

@johnsonshiue wrote:

I suggest you look into Fusion 360.

---

I will make significant wager that the experience will be no different in Fusion 360.

I recommend requesting example files and then showing actual demonstrations.

[dxmv]

1. I make models for scenery. In the next step, they go to the cnc machine

2. If by equipment you mean a computer, it's a pretty powerful system! Believe me!))

[dxmv]

1. I don't have 1000000 curves!)) It's interesting though, a model with good detail is an interesting model.
2. of the many simple sketches are simple details, but when it comes to ornamentation, this way takes a lot of time.
3. Of course! That's the way it is now.... Part of the work has to be done in Rhino, then export to Inventor and refine... But I want to do the whole model in Inventor!) And if you add in Inventor plugin Grasshopper, finalize and make comfortable function Sub-D, add the ability to work with multiple curves - and generally will be super Inventor)!

[dxmv]

1. I have every element carrying the intent of the project! It's just not always an engineering intent. There is also the artistic intent of the project).
2. Fusion 360 - same story ((
TSpline needs improvement (in my opinion).
TSpline needs to be as convenient as in Rhinoceros! (what can be easier, you just need to repeat the mechanism that works...)

[dxmv]

1. I agree! Fusion 360 is not considered Fusion 360 is not an option!
2. What files do you need?

[pcrawley · Accepted solution]

Where did the artwork come from?  I'm guessing it's a 2d vector file from a 3rd party application.  Can you save it as DWG format?  If so, there's a workflow that will speed things up.

Why is it slow?  The sheer number of line segments and constraint assumptions is what's causing the delay with your existing workflow.  The sketch solver is attempting to solve thousands of coincident constraints - and probably more of you attempt to edit anything.  The idea of the sketch solver is to solve sketches with geometric constraint assumptions and dimensions, whereas your sketches are artistic and don't suit that process.  You can however bring the sketches in without all that baggage.

On the 3d Model tab (in a part file), find "Import" (in the Create group) and select the DWG vector file.  It can be as complex as you like.  Note that you need to select a plane to put it on, and a point to reference, so I suggest projecting in the origin.   The Inventor origin now becomes the world 0,0,0 point from the DWG. 

Once imported, you create a new sketch, and tucked under "Project Geometry" there is "Project DWG Geometry" that has options for "Single Geometry", "Connected Geometry", and blocks.  If you try "Single geometry", you can window-select the DWG vectors.

The imported DWG doesn't contain all the center marks for arcs and circles, so it doesn't look like a PhD-level dot-to-dot exercise.  Unfortunately, as you project geometry through to the sketch, those dots appear.  However, because it is simply "Projected Geometry", no coincident constraints are assumed or added - so it is fast.  Note that the DWG is associative, so editing the original DWG will update your projected entities in the sketch.

I once had to import a 2d drawing of a tree with a thousand curled leaves (all splines), and the whole shape had to be profile cut from steel plate.  Your existing method cost me 2-hours, but then I tried the DWG import process, and had the job complete in about 15 seconds.  If you love Rhino for curve editing and creating artwork, carry on - just export the curves to DWG to get them into Inventor.

And for those who are constantly throwing Fusion into this forum as the answer to anything vaguely difficult, there's a whole bunch of Fusion forums to play in over here: Fusion 360 - Autodesk Community  

[dxmv]

Yes, thank you so much!)) It works and it really is faster! Question for you - how do I remove all the projection dependencies "in one click" after I have projected all the desired geometry from the DWG file (I understand that I can edit the DWG in AutoCad or Rhino and all the changes will show up in Inventor)? I did the illustration myself. I made the curves in Rhino. The thing is that except for DWG no other way to work with ornament in Inventor. Why it is slow in Inventor - I know and in general I know the solver algorithm... I do not understand why there is still no possibility in Inventor just turn off the solver (in cases such as mine) ...? And pure geometry and artistic ornamentation is a creative process, there should be no distinction (in my opinion)! As for my love for Rhino or Inventor or any other software - I don't really have a love for software!)) For me software is a means (a tool)... I distinguish them by - comfortable to use or not comfortable to use, necessary to use or not necessary to use, etc.

[JDMather]

I have seldom done this...

Excellent.

[pcrawley]

@dxmv - I can help you there too.

Window select all the geometry - now all the projection constraints should be visible.

Right-click - "Delete Constraints"

Done!

Thank you @JDMather.  I use that plenty with your posts.

[Shag_Bore]

Hello @pcrawley !

I have a question regarding your method for dealing with vector images. We are a sign company and use fonts and logo's all the time. These get routed out or cut on vinyl use dwg or cdr exports. That end of the system works fine. 

I run into trouble when trying to find a way to show the design in Inventor for fabrication drawings. I was doing it the painful way of inserting the dwg into a sketch and reconnecting/constraining lines and endpoints so that I could extrude the profiles. takes hours and millions of clicks.

I was happy that I found your post of importing the dwg directly then projecting dwg to new sketch. But I run into this issue of the projected lines becoming "wavy" The dwg shows the lines being straight and square. I am not sure why after the projection they change. 

Our graphics department utilizes CorelDraw and Illustrator, maybe there is an option they can use when exporting to prevent this as there doesn't seem to be any options to work with in Inventor. 

Here is the waviness I am speaking of. Black lines are imported dwg files, green lines are the projected dwg geometry .

thanks!

[pcrawley]

Hi @Shag_Bore - any chance you can post the DWG?

From the image, it looks like Inventor is connecting some elements as splines.

[Shag_Bore]

Hey @pcrawley!

here is he dwg that I used.  Hopefully you can find something!

Thanks

[pcrawley]

It looks like my guess was correct - the geometry in the AutoCAD file is all splines:

Assuming you have a Product Design Collection, you'll have a copy of AutoCAD.  You can open the DWG in AutoCAD and convert the spline to a polyline using SPLINEDIT.  There's an option to turn the spline into a polyline and reduce the number of vertices:

After you hit "convert to Polyline", enter 1 for the precision (this should reduce the number of vertices to something manageable in Inventor).  Save the DWG and try the Import process in Inventor.  Even with the setting at 1 (its valid range is 1 to 10) the number of vertices is still very high.  If this was my job, I would probably trace the imported geometry in Inventor, then delete the imported sketch.  (High vertex count in an Inventor sketch = sluggish performance.)

An alternative method would be to ask if Corel Draw/Illustrator can export as "AutoCAD R12/LT2 DXF files".  That version of DXF didn't support splines, so it automatically replaces them with polylines.  Bring the DXF into AutoCAD, save it as a DWG, then try the import process to Inventor.

As a final question - which I should have asked earlier - which version of Inventor are you running?  Your DWG imported and projected perfectly in my Inventor 2024 (although the vertex-count is unnecessarily high!).

I'm not sure if this is deliberate, but almost all the straight lines of the text have a tiny "chamfer" at the end of each line.  Some are more pronounced than others - I couldn't spot any pattern - they're seemingly random.  It might be to do with the spline coming from the source application - or the interpretation by AutoCAD.  I'm only mentioning it in case those corners are supposed to be 'square' - I'd hate for you to discover further down the track!

 

It's not as clean as I'd hoped - but I hope this helps!

[Shag_Bore]

@pcrawley wrote:

As a final question - which I should have asked earlier - which version of Inventor are you running?  Your DWG imported and projected perfectly in my Inventor 2024 (although the vertex-count is unnecessarily high!).

---

Another item to add to the list of arguments for upgrading, I am still utilizing 2016 right now.

---

@pcrawley wrote:

An alternative method would be to ask if Corel Draw/Illustrator can export as "AutoCAD R12/LT2 DXF files".  That version of DXF didn't support splines, so it automatically replaces them with polylines.  Bring the DXF into AutoCAD, save it as a DWG, then try the import process to Inventor.

---

 This option partially worked, I got the graphics designer to export to dwg R14 and dxf R14. The dwg r14 still imported and projected the wavy lines. I tried opening in AutoCAD 2016 and saving the dxf to dwg but again, wavy lines. However if I import the dxf into inventor part sketch directly, the sketch doesn't become wavy. I unfortunately have to run sketch doctor to close loops and fix what it can. It does delete some curves as it tries to "fix" the sketch with overlapping lines. Not perfect, but still cut time spent dealing with this, and it seems less stressful for Inventor which also makes it faster. Also importing the dxf directly to part sketch doesn't allow me to project dwg geomtry to new sketch. 

I don't know too much about CorelDraw or Illustrator, how the designers create the text or logos, I am not sure why small chamfers like that would exist. Maybe they come from the font they use? 

Thanks for now @pcrawley !!