Converting a sheet solid to a close solid body

[dmaier]

I have imported a step file from proe that has several gaps in it.  As far as I can tell there are no gaps left after converting the solid to a surface, creating the missing surfaces, and converting back to a solid. I am left with a sheet solid. How do I convert this to a closed solid and or verify if there are no gaps left.  I wish to cut the part by a plane to create a better cross section view for presentation and do not wish to have a hollow inside of the part.

[Colin Gilchrist]

Just because it is a "Sheet Solid", does not mean that you'll have a "hollow wall", as if you performed a "thicken" operation. You should still only get a single intersection of the "outside surfaces" of the sheet solid, when you Slice the model with a Plane.

[dmaier]

Other than a simple shape like a cube I have never got the thicken operation to work. All I get is an error stating that the thicken operation failed. Is there more to the thicken operation than selecting the solid, a direction, and amount to thicken by? 

[huskermcdoogle]

Do you have ProE/Creo?  I so export as a different format if you can.  Otherwise you will need to go through and change a bunch of settings to get a decent step export that mastercam will like.  Makes all the difference in the world.  Let me see if I can dig up the settings needed for a decent step export.  If you don't have it, send the recommendations along to the customer and have them export to these rules and you will almost never have a crappy non-watertight model again.

Can't seem to find the post from back in the day that well explained the settings that need to be changed. I'll look later.  IIRC Murlin was the one who posted them.

[dmaier]

It would be great if you could find the export setting to get a mastercam friendly step file. I will try looking myself as well. I do not have ProE access any longer. Kinda feels like I have my hands tied behind my back now when I have to do anything involving editing a 3D model.  

[huskermcdoogle]

On 2/23/2010 at 2:18 AM, Watcher said:

Hi everyone!

 

There are many Pro/E configuration options to configure model export. I could not list them all here... However I´m open to help anyone who wants to dig deeper…

One of the biggest problems that occur with Pro/E is that it works with two types of accuracy: Absolute and Relative. In a nutshell, Relative (The default) varies the accuracy of the part based on the model size among other things. Big features are less accurate than small ones. You do not have this concept on most CAD systems and probably Pro/E is the only CAD/CAM system that works this way. Accuracy mode has a huge impact on the way Pro/NC handles toolpaths for example... There is a reasonable reason for the two modes: Absolute mode forces Pro/E to consider the same accuracy for all features in the model, from a tiny edge to a huge curved edge. This increases the model size substantially and this is the reason why it is not enabled by default. As the accuracy varies, the topology/geometries of exported models are also affected. This works fine in Pro, but other systems out there do not see it this way. This option is only activated through the config option enable_absolute_accuracy = yes – It enables a hidden option.

 

There are a few other settings that affect model quality and export accuracy:

 

enable_absolute_accuracy = yes

 

step_export_format = ap214_cd

 

accuracy_lower_bound = 0.0000001 #this is very important option for model export. And yes, the value is very smaaaaalll.

 

default_abs_accuracy = 0.00003937 (0.001mm)

 

iges_out_trim_curve_deviation = 0.00003937

 

intf3d_out_surface_deviation = 0.00003937

 

After setting the option enable_absolute_accuracy = yes you will see a new option in the modeling environment: Go to the menu "Edit" > "Setup" > "Accuracy" : A new option named "Absolute" will appear. Set the absolute accuracy you want. The model will be regenerated. To set small tolerances the option accuracy_lower_bound must have tiny values.

 

If the part is complex and it was originally designed using the default "Relative" mode, you might experience problems during regeneration because now Pro/E mathematically sees the features, specially the small ones as they really are: tiny. So some references may get corrupted.

 

There is a very good explanation regarding Absolute vs. Relative at PTC website, but I´m not allowed pasting it here since it is copyrighted material for active maintenance customers.

 

There you are going to find the formula Pro/E uses to set the relative accuracy for each geometrie.

 

Most people don’t use these settings and if you are not using Pro/NC as well, the default settings cover 90% of the cases. So this is a good source of problems regarding Pro/E and model export problems.

 

After using these settings, don’t forget to set smaller tolerances for model export in Pro/E whenever this option is available at the export dialog.

 

JM2C,

 

 

Give this a shot, some of the settings may have changed a little over the years, as I recall it was a little different in creo2, but generally the same idea,

[dmaier]

Awesome, thank you. Hopefully this will save some headaches importing files.

[huskermcdoogle]

Usually helps portability going to any system.