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problem trying to import a dxf file of a simple gear to extrude in inventor 2013

3 REPLIES 3
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Message 1 of 4
Gargole
1372 Views, 3 Replies

problem trying to import a dxf file of a simple gear to extrude in inventor 2013

Hello,

 

I just started learning inventor and tried to make a first sketch and use import acad file. I have a simple gear in dxf. It took some time to show up in the sketch. When i selected the gear inventor freezes. I closed the sketch to make an extrusion and inventor freezes again.

 

I originally started with inventor 2014 and had same problems. So decided to do a step back to 2013 thinking 2014 was too heavy for my pc.

 

My pc is a i7-930 3.2ghz with 6gb ram1600mhz and win7 64bit with a ati radeon 5970 gpu. i installed service pack 1 and 2 and all other updates for 2013.

 

I think my dxf file is the cause. Its made out of all little lines/curves etc... btw in rhino i have no problems extruding this dxf at all.

 

Must i do something to clean up the dxf first for importing to inventor?

 

Could someone shine a light on this? Thanks! Appreciated.

 

I attached the dxf where its all about. The second dxf i have the same problems. When imported and try to work with it inventor freezes/becomes super slow and says not responding.

 

 

3 REPLIES 3
Message 2 of 4
Mark_Wigan
in reply to: Gargole

yep Gargole, you are onto it...

 there are many small elements that inventor is likely constraining for you (default option).

 

so, you can choose at time of sketch import what you want inventor to do. Just have a bit of a look at the options / check boxes in the import dialogue box before you click ok. i would suggest turning off all of the constraints to start with. see how that goes. (for me, usually just asking for 'constrain end points' is sufficient). then after the import, finishthe sketch. do not try to mess with it, move it etc. *

 

ps- in autocad, run the 'overkill' command prior to export block / save. you can minimise the amount of  data before you begin. also, pposition the autocad / dxf geometry onto the 0,0 origin point, so that when you bring it into inventor, it is sitting at 0,0 for you.

 

 i would also consider make a autocad block before you save the drawing. then, at time of import to inventor, you can choose ' make autocad blocks into inventor blocks' . that way you dont need to constrain it, and, you wont need to worry about the sketch going crazy if you accidentally touch it after import.

 

note- you may like to investigate the inventor tools for creating gears and other machine parts via the Design Centre environment. they can be generated automatically simply by your input of several pieces of information.

 

hope this helps.

 

best regards,
- Mark

(Kudo or Tag if helpful - in case it also helps others)

PDSU 2020 Windows 10, 64bit.

Message 3 of 4
SBix26
in reply to: Gargole

You've just got your first lesson in the differences between AutoCAD and Inventor.  This is a really poor way to model things in Inventor, and the reason is that Inventor maintains relationships between things, such as sketch entities.  If you look down in the lower right-hand corner of your screen when editing the sketch, you will see a number indicating how many dimensions are needed.  I imported the dxf file with end-points constrained (as Mark recommended) and my sketch now shows that I need 14024 dimensions-- that's roughly how many degrees of freedom this sketch has!  Mathematically, you can start to appreciate why this sketch, though simple in AutoCAD, is not in Inventor.  You may also try to imagine placing 14024 dimensions and contraints...

 

A much better way to model this would be to start with a plain disk, cut one tooth profile, then pattern it.  Cut one of the six openings in the interior, then pattern it.  Place the hole in the center.  Extrude the keyway.  Finished.  The features can be done in any order, but be sure to use the Origin features to constrain everything to.  All sketches should end up 'Fully Constrained' in place of 'n dimensions needed'.

 

You might start by going through JD Mather's basic Inventor tutorial: http://home.pct.edu/~jmather/SkillsUSA%20University.pdf



Sam B

Inventor Professional 2015 SP1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M

Message 4 of 4
Gargole
in reply to: SBix26

Mark and Sam,Thank you for expaining this!

 

My noob mind thought i just could simpel import it and extrude it. i shall look into it to create a plain disk and pattern the tooth. For now i think im starting with just the basic lessons and forget about importing my gear for a while :).

 

Thanks for the lesson link!

 

 

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