bad representation of sections in 2d drawing

[D'Amato_A]

good morning

I have a problem in my Creo version 7
when I create sections in the presence of imported objects the sections show lines that should not appear

I need to work with objects imported from Step and Iges of a fair amount of complexity. Therefore I cannot fix the errors and I let broken solids and surfaces be created.

In the images that I post below the view from 3d is shown in "no hidden" view and the section of the 2d model, as you can see the section shows the objects as if they were in "wireframe" view

In the definition of the "view display" view it is marked "no Hidden" and it is actually like this for all the solids of the drawing that I created, but not for the imported objects

In the definition of the "section" view by selecting model edge visibility>area the section correctly shows only the sectioned volumes

I definitely need to solve this problem because in some sections it is not possible for me to work

correct view in 3d section

bad view in 2d section

  

thanks for reading.

post edit

select "include quilts" in the definition of the section remove all the quilts, and that is bad because remove also object that I want to keep

[StephenW · Accepted solution]

Because it's purple in the drawing, i can tell it's a surface model (quilts)

Go back to the model, edit the section view, under the Model tab, click the "include quilts" button

Then in the drawing view, edit the view properties, under the view display tab, click the "HLR for quilts"

[D'Amato_A]

thanks for the reply
i did. it does indeed remove the purple lines. however it works too well: it also removes the surfaces of the objects that have not been sectioned. effectively removing half of my objects from view.
which makes my section as useless as before

is there no way to discriminate which components to preserve?
include and exclude components in the section definition does not work

[StephenW]

Your x-section should cut thru the solids and surfaces at the location you set. Likely you are expecting the surface model to section like the solids. 

I'm just guessing here but you probably need to work on your import model so it's a solid, instead of a surface. It's just a guess, I really have no idea what you are asking.

[KenFarley]

You said that you did not fix parts that had "broken" surfaces and the like. Therefore, Creo can't cut sections through them; that only works with manifold solids. You need to, as Steven suggests, fix the models you imported so they result in a solid object. Otherwise, the sectioning algorithms have no idea what is "inside" or "outside" the part, etc. This is why I often have to build a simplified model of something instead of using a complicated model obtained from a supplier. They often like to use molded-in text, multiple intersecting objects, etc. that make it impossible for Creo to build a solid model.

Regrettably, the only tool I know of to fix these models is the Import Data Doctor. It's very useful, but often quite tedious to use.

[StephenV]

Good to hear some suggestions worked but unfortunately too well. I then investigate from there since something seemed to make something happen. I looked at other responses for your situation and these folks are on top of things with their suggestions. Use them! They are things I have done in the past too but I could not explain as good as these folks did. It's been so long ago. Accuracy settings, export model settings to tailor towards resolving your issue, and more. That Doctor thing does work well but as said, "tedious".

'May the Source Be With You!!'

Stephen V

[D'Amato_A]

@StephenW 

what I would like to get is a 2d view as if it were a 3d section view "no hidden"
the 3d one works correctly
but when you bring everything to 2d Creo fails.

@KenFarley , @StephenV 

unfortunately I work with Step files of the size of one or two GB with a final count of parts that varies from 5000 to 30000 components.
In the Step assembly there are objects that have dimensions of several meters up to the screws and bolts.

Of this assembly I make a simplified view and then export everything as Iges.
In order to have the assembly as a single lighter component.

Healing the geometries not generated correctly is out of the question unfortunately

among the possible solutions that I found:
a- generate two different views, one in which the section includes the quilts, one where it does not
convert the file to DWG and refine the drawing in native 2d software

b- generate the section view where I do not include the quilts, export everything to dwg and export generating the groups of components and views (see image)

in this way a group will be created for each single component in each view (suffering). the "sick" surfaces will not be included in the group and therefore will be easy to select

c- Create simplified models to replace the geometries imported incorrectly by tracing the sick surfaces and work a lot with the simplified representations

Anyway, you were very kind in responding promptly and helpfully. Thank you, so much!

[StephenV]

Hi,

I'm responding in a quick moment and I might not be helpful here but from past experiences in many CAD (mucho PTC) xfers and such, go and seek where these extra lines or phantom geometry lies in LAYERS. You can turn on/off and manipulate stuff in layers.

When importing see if there are more places within the import process to manipulate what your bringing in (it's been a while for me).

Good luck.....sorry can't research it now and just throwing out thoughts to see if it helps.

[D'Amato_A]

Hi

I have never been able to understand how to use layers effectively. There are simply too many of them and during export-import the layers can be hidden or deleted one by one, but this does not affect the geometry, leaving lines and/or edges present and hidden.
every now and then they reappear on 2d out of nowhere for example welding.
not being able to make them visible again on the model I cannot delete them

[kdirth]

As for improving importing results, there are several things you can do in the import settings to get better results.

• Set Model accuracy to external. If you impose a conflicting accuracy on the import, it will likely have issues because the math does not work. It has also been suggested to me to change the part accuracy to that of the import file if known before importing.
• In the topology tab, Uncheck Heal options, set Join surfaces from the same layer, group, or shell to yes, and set Solidify closed volumes to yes.
• Other settings may help also, but those are the most helpful.
• I also always use "Use templates" in the model tab.

When you determine a set of import settings that work well for you, select save profile and set the corresponding config in your config.pro to use the saved profile.

[D'Amato_A]

Hi
I will try to improve the import as you suggest. However I can't make many attempts because the Step files I use take hours to generate.
In case could you point me to a post where it is explained in an exhaustive way how to improve the setting for importing large step files as much as possible?

[StephenW]

I work with large assemblies all day, every day. If you are exporting models and then bringing them back in again, but you still need fine details of those exports, your method is likely going to cause you lots of pain. I sometimes use a similar method to help simplify my models, but ONLY on areas that I don't need fine details and areas I don't need to worry about changes on the other parts/assemblies.

If you are working with large assemblies, you need to utilize simplified reps to reduce your detail and possibly envelope parts.

You may also want to look in to shrinkwraps for simplifying components.

Large assembly management is always a challenge. There is a PDF in this thread https://community.ptc.com/t5/PTC-Community-Networking/Bringing-Large-Assemblies-Down-to-Size/m-p/444618 done by Steven Lapha. He explains some of how NASA is managing their large assemblies

[D'Amato_A]

thanks, I will definitely read it and I hope it can be useful to me.

My company develops industrial plants.
We are many different offices and we in particular for historical reasons are the only users of Creo.
For this reason when we have to develop a new installation we have them send us the step generated by their general assembly and then we simplify it.
Therefore I do not have the possibility to intervene on the export settings.
The general assembly that they send us is heavy and is composed of a mix of models from multiple offices, from those who have finalized their component and therefore the threads are also represented, to that only sketched model, perhaps in shrinkwraps

the problem is not the model. It is that then of what I develop I have to produce an installation drawing that potentially reaches the customer, so it must be fairly acceptable.

Thanks again for the answers!

[StephenW]

This makes a lot more sense. It's always difficult to imagine the details of why a user is doing what they do. We also have different groups using different software. It can be challenging sometimes. Luckily most of the groups I get components from use Creo. 

For importing, pay attention of kdirth's import recommendations above. We use the accuracy set to extrernal also and that solve many of our problems. If you use windchill pdmlink, it is also sometimes beneficial to do the imports when disconnected from PDMlink for both speed and getting the model to solidfiy after import.  Unfortunately, there is no one-size-fits-all import solution for importing models. Sometimes I will test an import in solidworks and/or inventor and if it has more luck importing the solid model I will try to re-export those models to improve my Creo import.  Lots of trial and error!

[kdirth]

You may want to look into receiving and using the native files of the other offices.  Creo is capable of opening files from many other CAD programs.  The models will still solids without the underlying data (modifiable features), but should be a lot better that an imported STEP or IGS.

[D'Amato_A]

@StephenW 

we don't use a PDM, we are very order-oriented and the little that we reuse we can currently manage manually, almost XD.

kdirth, I admit that I didn't know I could open files from other software, no one in the office at this point I dare say.
It will be interesting to discuss it and see if we can save a lot of time.

You made me discover many new things. Thank you all, really!

at this point should I close the post or will it close by itself?

[kdirth]

If there is a post that best solves your issue you can select "accept as solution" to let others who find this thread in a search know what helped you the most.

The post does not actually "close" until it gets old enough (years) at which point it is locked.