Drawing vs 3D CAD Model 1

[Twullf]

I have a model that will have to be cast, but it has some very complex shapes. Using Unigraphics, I am unable to get a radius into a region I KNOW they are going to need it, the program just will not put the radius into it.

So here's my question. The Model will be sent to the customer along with a drawing. If I call out a larger radius on the drawing than they find on the 3D part, will that supersede the model? Or should a notation be included on the drawing to indicate that the larger radius is prefered regardless of what the model shows.

Unfortunately due to the complex geometry of the part the Model has to be provided as well as the drawing.

Thank you for your time,

 

[looslib]

Put a note on the drawing stating: "Model provided is to be used for producing the casting due to the complex shape". Or something similar.
If you can't get NX to give you the radius value in a dimension, then you may have a generated a shape from blends that is not a true radius, but a curved surface. Have you tried doing a cross-section at the point you want to dimension the curve at?


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[HGMorgan]

In today's CAD world, the 3D model is the configuration control master, and, if there is a drawing, the drawing consists of views from the 3D model.
They should match, period.
Actually, I think you have a bigger problem than the old Model vs Drawing battle.
If you can't get the model to the configuration you want, how could anybody make the configuration you want?

Harold G. Morgan
CATIA, QA, CNC & CMM Programmer

 

[CheckerHater]

Who are "they" in "they are going to need it"?
If it's manufacturer, make a note like "RADIUS X.XX IN THIS AREA PERMITTED"
If it's customer and radius is functionally required, make your best effort to model it like looslib suggested.
Either way make sure the note will be noted. Many shops tend to ignore the drawing, go purely by the model, and refer to the drawing only after something goes wrong.

 

[ctopher]

I agree, make them match.
If the drawing is going to have changes, and not the 3D model, might as well use ACAD.

Chris, CSWA
SolidWorks 14
SolidWorks Legion

 

[Twullf]

To clarify, I think it is a problem in how UG determines a radius.

The geometry is a constantly changing shape. I am able to get most of the draft angles and radii in, but in the location indicated by the picture the coding of UG is not permitting me to put a large enough radius, and it is failing inside the circle. I believe in practice this problem is non existent and the manufacturers would prefer the radius and it would make their job easier, but I am spending hours trying to get UG to do something it is failing to do.

What I am getting from the conversation is that the model HAS to be right and that the drawing is only present in case of problems or to provide the person receiving the part elements they can check.

Which puts me in a quandary as to how to solve this problem. *sigh*

Unless someone knows a good say to use documentation to allow the manufacturer to put in the necessary radius. I'll take this to the Siemens forum and ask for solutions on the UG side.

Thanks again

 

[ewh]

...might as well use ACAD

How much experience do you have using NX? Have you exhausted all of the different approaches you can take to create this radius, or just the blending commands? While it may take some time and effort, if you can draw it you should be able to model it.
I have never worked with a solid modeling system where the drawing was the master definition; it is always the model.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[ewh]

I was typing when you posted...
Is it a constant or variable radius that you need? Have you verified the integrity of the surrounding surfaces in that area? NX should be able to do this with a little investigation. It would be a good idea to pick the brains of those in the NX forum.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[TheTick]

There are lots of ways to attack this in 3D. There are many ways to define fillets:
[ul]
[li]Edge fillet (used 99% of the time)[/li]
[li]Face fillet[/li]
[li]Fillet to edge or line[/li]
[li]Variable radius[/li]
[/ul]

 

[Twullf]

I have been using Unigraphics since 2008, I have over 20,000 hours in the seat. Though with NX 9, which we have only just gotten I only have about 400 hours in the seat.

I have used ever option, including trying to use my own sweep sketch, but they won't join, and due to the complex geometry it isn't tangent to the two surfaces. The edge is moving in all three dimensions, and the angle on the seam is constantly changing as well. It is simply beyond the capabilities of the program as far as I can tell. And because part of the Siemens company and my company work in the same field I'm not allowed to send our models to them for help.

So yeah, that's where it is at.

 

[ewh]

That's a good amount of time using the software. >50,000 hrs myself, but I have yet to experience NX9.
Sometimes in situations such as this you have to go back and recreate the surface elements that are giving you problems. By doing so, you may find slightly different approaches that allow you to proceed with the radius in question.
Again, ask on the NX forum... I have been ever thankful for advice received over the years from its members when I have come across similar problems.

“Know the rules well, so you can break them effectively.”
-Dalai Lama XIV

 

[cowski]

I'd start by looking for discontinuities between the faces circled in your pic.
The 'examine geometry' command may also be useful.
Have you tried the different 'overflow resolution' options within the blend command?

 

[KENAT]

1. As ewh says have you tried surfacing or similar? In NX little brother I sometimes had to go back several steps and change order to get this kind of thing to work when surfacing so I have some appreciation for your frustration.

2. Are you being forced to play the purchasing 'telephone game' or could you actually talk to the foundry about your issue?

3. On the drawing if you have a call out for that radii generally just make sure it is clear that it's "ALL AROUND" - perhaps even adding that to the drawing.

The casting house is probably going to do some work on the model anyway to allow for shrink etc. so it may not be a killer.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[Twullf]

Hey cowski,

Yes I've tried the different overflow options. And Examine Geometry either Passes everything or there are no results. (I have never found Examine Geometry very helpful)

I can get a radius so long as the value is smaller than .3 mm, and no casting, scratch that, no cost effective casting will be able to maintain that.

 

[Twullf]

We are designing this for a customer who will source it. I have no contact with the supplier as a result. So I have to make the drawings / model as clear as possible.

Thanks for everyone's help by the way.

 

[KENAT]

OK, so put in a .3 mm radius and apply an appropriate tolerance in the drawing that covers what the foundry will want (while meeting functional requirements...).

While having the model ready for the foundry to take with minimal effort/matching the drawing... are good general practices at some point the effort (i.e. $) to achieve that may not be warranted.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[btrueblood]

I agree with Kenat. Let the drawing define the acceptable range, and move on to the next design. In the real world, where I work, I get paid to put parts on the shop floor, not to create mathematically perfect CAD models. CAD does not define the part, the purchase order does, by specifying whether drawing or CAD file takes precedence. At least, that's what the lawyers say.

 

[TheTick]

Hard to tell from just a picture, but there are some indications that the principle surfaces have some funkiness to them. Fix that, and your fillet should happen.

Time was, UG would allow users to adjust Parasolid tolerances. Tightening tolerances on the preceding features and loosening them on the fillet might get you there.

 

[jassco]

Hi, Twullf:

I took a quick look at the picture you posted. Something like this can be done with surface modelling.

If you post a section of this model, we can give you some suggestion.

You need to take a different approach as your current one leads to invalid geometries.

Best regards,

Alex

 

[ajack1]

I am intrigued as to why a designer with 20,000 hours experience on a high end CAD system feels that a machinist or whoever picks up the part to be made is going to be able to fix a model that they cannot?