Hole table on a STEP file

[xavier_dumont2]

Hello,

I have a STEP file that I import into Inventor.

I create an IDW on it and try to create a hole table. But all hole coming from the STEP are ignored. Is it a limitation?

Thanks in advance.

[Anonymous]

You would need to model in Inventor in order for hole tables to work, the information required is extracted from the hole features. .stp files have no features.

[JDMather]

Extruded circles would be ignored as well as they are not Hole Features.

If you are on subscription, you can download the Feature Recognition add-in to rebuild the feature tree to translate the imported geometry to Hole Features.

[srobert]

Extrude features are recognised, it's why I'm asking myself why STP holes are not recognised. I can add a dimension on it, then the diameter information exist.

But other information like depth, I'm 100% agree, this is not an existing information in the STP.

I got the same idea regarding Feature Recognition. But it's very heavy to use on the kind of part I need to recognize (plate for high complication watch).

[JDMather]

Oops, I didn't test this. 

When using Feature Recognition - I only use on those features that I actually need.

https://apps.exchange.autodesk.com/INVNTOR/en/Detail/Index?id=appstore.exchange.autodesk.com%3aFeatu...

[xavier_dumont2]

Then, I understand i'ts a limitation of Inventor.

PS: Oups sorry for the post under the name srobert. I don't realise that I was connected withg my collegue account.

[jalger]

Hi Xdumont,

If you use the Feature recognition tools it works fine. I used the Auto recognition and it discovered the holes properly

The XD1.stp process the holes properly for 2014 and 2015, so I'm not sure where the limitation is? (did you run the tool and have it fail?)

If you have more than 100 Features that are being Detected, its probably a good idea to recreate the part (and use a pattern). I have had it work with more then 300 features (Took forever to process though).

If you have the full model with all of the holes, try the tool manually, my suggestion is to recognize no more then 20 features at a time let it calculate the solution. Maybe post the full file on here for us to try.

JD Posted the Exchange site for the Feature Recognition tool.

All 3rd party data comes in as a dumb solid when importing. This is true for any design software, its the whole proprietary thing, Autodesk won't  share its modelling engine with solidworks,  Solidworks won't share theirs with Autodesk... and unfortunately it leaves the average user needing both programs to do full edits for both file types (sldprt vs ipt).

Note: you could use fusion to have free form design changes (deleting holes and adding/removing other things), but even bringing it through there will not cause a step file to magically map the hole features.

Attached is the result from running it through Feature recognition (its 2015 file format).

Regards,

James

[JDMather]

---

@srobert wrote:

Extrude features are recognised,...., then the diameter information exist.

...

---

An Extrude Feature or a Hole Feature has very specific meaning in Inventor, SolidWorks or Creo.
The history tree must list the feature.

Just because you can measure a diameter does not make a feature a Hole feature.

[xavier_dumont2]

First of all, thanks for your time. I appreciate.

The file I attach to my original post was a just a simple sample to show that holes coming from a step are not recognised.

I can't share the original part file because it's a customer's parts (I'm working for an Autodesk reseller).

I try an automatic recognition but only 90% of holes are recognized (but it's better than the first release of this add-in on Autodesk Labs).

I try manual recognition but some holes are partials, then no way to transform them into a hole feature.

Just to have an idea of the part, it's somethings more complicated than this (both side are like the face you can show on the picture).

http://s83.photobucket.com/user/VINGOXF/media/PlatinesEP.jpg.html

Many holes are partials because other holes or extrusions are eating side of the hole.

It's not only one part, all development of this customer are in step (other 3D cad software). Actually, the only solution is to use our own tools in order to create a coordinate/hole table in IDW (this tools recognised the curve object in the IDW and get the diameter value, no matter of the kind of feature), but I always try to find other solution to propose to our customer. I will propose him the feature reco add-in as an alternative.

The hole table feature is a tools who don't evolve from years. There are many things to do to improve it, I will open an idea for that.

Thanks again and have a nice day.

Regards

[AVIDC2AC]

Question,

I had no idea this tool exsisted and it works great when 1st importing the Model.

My question is If I have already saved the STEP file as a IPT, I cannot seem to find a way to activate the feature recognition.

Is it not possible to use this tool after a file has been converted and edited in any way and saved to an IPT?

[JDMather]

Right click on the base solid node.

[AVIDC2AC]

Doesnt work, guess its a limitation of this tool, still cool tool, thanks for the tip JD

Test for yourself, import a part make any change even a direct edit save it open it RMB on the Base and the menu option item is gone.

[JDMather]

I am not at my Inventor machine right now, but what happens if you roll up the EOP?

[AVIDC2AC]

It still doesnt work, the only way I was able to get it to work is if I did it on a "Standard Partl".

The file I had was a Native Solidworks Sheetmetal file which I converted and It comes across just fine. But, when you convert the part to "Sheetmetal" in INV, you loose the option to use feature recognition. However, if you delete the Sheet metal feature or just Convert it back to a "Standard Part" then moving the EOP seems to work just fine if features were added or it just prompts you and says its gonna delete anything you made it doenst like.

So it seems the the issue here is directly related to the convertion of part to a Sheetmetal.

If im wrong let me know what it is.

And thanks again for your feed back

[blair]

Possibly try adding "Sketch Hole Centers" and then set the Hole Table to include Center Marks. This should bring in the locations (maybe).

[blair]

I thought there was something in the Autodesk Labs a few years ago that working within Inventor. It's been long retired, perhaps in might show up again within Inventor.

Currently the Feature Recognition only works upon the Import of Neutral files.