topic Re: Display of threads in exporting file formats e.g. step in Inventor Forum

Display of threads in exporting file formats e.g. step

Anonymous — Wed, 24 Jun 2015 10:32:43 GMT

Hi,

I have to export 3D drawings with threads for customers who needs other file formats.than Inventors .ipt

One asked for STEP, but when I have made the export and opened it in Inventor LT 2014 to check if everything is okay the threads were missing in the file. 😞

I found a post from 10.06. 2011 about this subject, explaining that STEP format dose not carry the thread information.

It also suggest to pecify the thread size, pitch and length. (I pasted in the post for reference, see blue text below)

How can I do this on the drawing?

Is there a way to show threads in the drawing, that can be included when I export to other formats?

I guess the customer wants to insert my drawing in their own exsisting drawing, but if the part includes a thread, how can they use it if they are using another software that inventor?

Is there any of the other 3D file formats available in inventor that can show the thread type in the drawing?

Re: Exporting STEP with threads?

10-06-2011 02:32 PM in reply to: es12

es12 wrote:
I have to export the drawing to STEP for machinist that uses Solidworks.

SolidWorks does threads exactly the same way (cosmetic representation). STEP does not carry this information. You simply need to specify the thread size, pitch and length - your machinist should be able to figure out the rest.

Please mark this response as "Accept as Solution" if it answers your question.
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Thanks in advance,

KBE

Re: Display of threads in exporting file formats e.g. step

JDMather — Wed, 24 Jun 2015 11:43:30 GMT

@Anonymous wrote:

How can I do this on the drawing?

Is there a way to show threads in the drawing, ...

I guess the customer wants to insert my drawing in their own exsisting drawing,

KBE

You seem to be confusing the terms "parts" and "drawings".

1. Create a 2D drawing with the thread notes and send that along (as a pdf) with the STEP,

2. model the thread rather than use cosmetic threads.

#1 is the more usual technique.

Re: Display of threads in exporting file formats e.g. step

mcgyvr — Wed, 24 Jun 2015 12:15:05 GMT

^^^ Yep.. We do #1 for all our outside sheet metal, screw machine, etc... vendors

The ONLY reason to actually model "real" threads is for 3D printing

A step file is not a drawing, its a 3D model

Drawing = 2D

Part/model/step/iges = 3D

Re: Display of threads in exporting file formats e.g. step

Anonymous — Wed, 24 Jun 2015 13:28:47 GMT

HI,

Thanks for yor reply.

Yes, I see, my use of the terms "parts" and "drawing" is not consistant, sorry

My question is regarding the 3D model.

I am working in inventor, but haven't tried the exporting feature untill now and thought the thread info would be included in the exported file as well.

Is best practise on this issue to deliver the STEP file accompanied by a 2D drawing (pdf) with dimensions including the thread notes?

thanks in advance,

Kbe

Re: Display of threads in exporting file formats e.g. step

mcgyvr — Wed, 24 Jun 2015 13:33:19 GMT

@Anonymous wrote:

HI,

Thanks for yor reply.

Is best practise on this issue to deliver the STEP file accompanied by a 2D drawing (pdf) with dimensions including the thread notes?

thanks in advance,

Kbe

depends on what you are doing with the file and what information the end user needs.

But yes STEP files do NOT include thread information nor any other information besides the actual physical model.

Part finish, tolerances, thread detail, etc... are not included.

So if you are sending this to a vendor to make the part for you they will need more information than what a step file can provide which is typically done with a 2d drawing included with the step file.

The vendor may use the step file for programming the machine and the drawing for any other information thats not included in the step file.

Re: Display of threads in exporting file formats e.g. step

JDMather — Wed, 24 Jun 2015 14:23:41 GMT

@Anonymous wrote:

...

My question is regarding the 3D model....

Kbe

...and if all of this is in reference to threaded holes - use the Hole command with Thread option to get the correct tap-drill sized hole in your 3D Model. I find it astonishing how many designers specify a Ø5mm hole for an M5 fastener.

Re: Display of threads in exporting file formats e.g. step

merismith — Mon, 09 May 2016 14:31:18 GMT

Can someone explain to me how to export my files to .stl that keep the threading? I am trying to print some sample parts for student projects and we cannot get the threading to carry through. I know it has to do with the geometry, but we haven't figured out how to get the geometry of the threads to carry into the .stl file.

HELP!!!

Re: Display of threads in exporting file formats e.g. step

JDMather — Mon, 09 May 2016 14:35:08 GMT

The default Thread features created by Inventor are only cosmetic representations (zoom in very very close - do you see any real cut threads?).

If you want to 3D print threads - you will have to model the physical threads.

Attach your *.ipt file here if you can't figure it out.

Re: Display of threads in exporting file formats e.g. step

graeme_robinson — Wed, 08 Jun 2022 08:26:36 GMT

Bit harsh that response, spread some positive vibes, makes for a happier day for all

I am looking into a similar proces, I have been exporting data to the customer as ipt and Iam. Now the sutomer has solidworks and when I export the iam file the fasteners dont have any thread information. Yes its an image, but there is a thread length,

am getting around it by doing a pack and go of the inventor assembly i am doing, then in the pack and go doing a 0.01 mm cut to show the thread in the fasteners on the inventor part, then sending the stp file to the custmer.

Granted there are abotu 100 fasteners but on about 8 different types of fastener.

then the happy customer can see if the thread lengths are exatly what he wants,

then when the design is all good and parts in manufacture the assembly pdf can be created.

all Good!!!