using a sketch in drafting

[tsjaikdus]

Is it possible to import a sketch in drafting? I've used this sketch to create the model and I need the exact dimensions in my final technical drawing. I've imported the model, but this proved extremely difficult to use. I've been editing (with basic curves) and deleting lines for several days now and the longer it takes the more it looks like this approach is going to fail. Basic curves are near impossible to match exactly over the model and most of the dimensions of the model are useless because of blends. On the other hand there's the perfect sketch. But it seems I can not use it...?

 

[cowski]

I don't have experience using sketches in drafting (though it seems like you should be able to); but if blends are the problem have you tried turning on virtual intersection lines in your view?

If you edit the style of your view there should be a tab that gives the appropriate options. I would suggest making them a different color and/or linefont to make them easier to work with.

 

[mjcole]

What you need to do is add the sketch to a Reference Set called DWG or just to your default reference set.

Most master model drawings just use a SOLID reference set which leaves out important features like sketches. You can retrieve the sketch dimensions using the Feature Parameters icon in drafting to get the original dimensions used for the sketch.

If you add the sketch to a reference set that will be the reference set for the model in the drawing, it is not possible to set a specific reference set for a view.

In order to be able to hide the sketch in views where you don't want it to display you can use visable in view and make sure the Layering is set to Original Layers that way you will have the solid geometry on a different layer and it won't be affected when the sketch layer is blanked.

If you want to display only the sharp corners you can add points to the sketch that will be added to the reference set.

Michael
Hope this helps.

 

[Shadowspawn]

tsjaikdus,
I'm not sure I'm following you. I'm understanding you to say that you import the model into the drawing in order to utilize the 'sketches' for your dimensioning. Is this right? If so, well....
Doing this totaly negates the 'master model' concept and all the benefits that go along with it. Too much to list here, but suffice it to say that this is a bad thing.
In a nut shell, what I think your after is a means of getting the model sketches to show up in your detail drawing to ease your drafting pains. This it totally possible without importing the model into the drawing or having a the model and drawing in the same part file.
What I'd suggest is to utilizing the 'insert feature parameter' thingy where your sketch dimensions are linked to your drawing. This, in effect, imports your sketch dimensions onto your drawing sheet (for specifics, check out the online docs, and from menu pull down in NX3: <drafting> <insert> <feature parameter> <follow the bouncing ball...>). This is pretty cool, but does have it's drawbacks. Primarily, if the sketch wasn't created with the detailer in mind (created as you will dimension it), the dimensions are pretty useless and takes a lot of manual effort to correct. Generally speaking, your always better off dimensioning from scratch instead of using this method, unless of course your making a template part or something to this effect...
Clear as mud?
SS

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[tsjaikdus]

Thinking about it, I actually want to copy parts of the sketch (part of the curves end lines in it) into the technical drawing and delete UG's default suggestions at those places.

Blends are part of the problem, but using virtual intersections won't do the job. Many blends in the model are too small, so the radius isn't correct and must be corrected in the technical drawing. Other thing is the fact that drafting doesn't want to put dimensions to many arcs and lines in the drawing. I don't know why that is. It just neglects lots of them that I thus need to trace with basic curves. The whole product is somewhat complicated and I'm now stuck in using those basic curves.

I know this is not a beautiful thing to do, and I don't like it doing it this way. But I don't know how to improve the model (I actually think it's rather ok) and even if I did know I doubt not having the same problems.

The questionable part of it is that the objective is to create mirror image of a well documented right handed product. My suggestion is really to scan the existing drawing into a computer and print out a mirror image of it. But for some reason they want a UG model (that they won't use for anything else) and a (non-parametric) drawing (with lots of basic curves corrections). Remarkable isn't it?

I'll try the suggestions tomorrow. Thanks.

 

[tsjaikdus]

Not much luck so far. For the most important sketch I get a 'null tag not allowed' error. Importing the less important sketch does work, however it also deletes all dimensions in the _modelling_ application (that is the dimensions in the sketch become invisible or unretrievable?).

 

[Shadowspawn]

tsjaikdus,
IF I'm following you correctly (which is doubtful...) your actually importing the sketches from one part into the drawing part, and detailing that?
If there's no way that we can talk you out of doing this, then why not just export out the 'curves' of the sketch, import them into the drawing, and detail those?

SS

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[tsjaikdus]

I ended up doing just that. But the sketch was completely parametric, so I regret I didn't know how to import those dimensions properly. However, importing the curves looks promising.

 

[Xwheelguy]

NX Drafting does not have a sketcher (yet) so there's no way for the software to maintain any constraints at all when you import the sketches. However, if you set up your reference sets correctly, you will be able to view the sketches (that exist in Modeling) in your drafting views along with the sketch dimensions. The intent of having this capability is to have the ability to edit your model via the drawing by editing the sketch dimensions that are shown in Drafting.

It sounds to me like he's wanting to flatten the views because he's trying to place dimensions on entities that most CAD systems will not recognize. For example, in the TOP view (XY plane) trying to dimension a radius that travels along or close to the Z axis. NX Drafting won't let you pick the radius because it's a face or surface, which most NX dimensions will not allow you to pick.

I'd just fake the dimensions with annotations and leaders rather than try to duplicate a model view generated in Drafting.

Then again, here we are with no visual references or anything, so we're all left guessing.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Xwheelguy]

And after thinking a bit more about this, I'm not so sure why he's even importing sketches....it's a waste of time unless the sketches are in the wrong plane to begin with. Just put your sketches from modeling on different layers by themselves and make those layers visible in the appropriate views in Drafting.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[tsjaikdus]

it's a casting. I've 2 really challenging sketches of both sides. Inbetween those sides is a complicated part that has blends and all that that aren't on the sketches. So 1) the part is to complicated to accept (all the) dimensions. And 2) the sketches are too simple to use by themselves.

I wasn't allowed to fake the dimensions.

 

[tsjaikdus]

so, hence the hybrid

 

[Shadowspawn]

tsjaikdus,
...but your doing just that by having a detailed print un-associated to the model. I've designed a lot of castings, as well as detailed my fair share of casting, machining, and cast/machining drawings in my day so I understand the difficulties involved, but I think your making things more difficult than they need to be.
To start with, I'm making the assumption that the model is correct. By this I mean that it passes all validity checks and is a valid solid body. Secondly, I'm assumming that you have standard cast size interior and exterior blends (.188 and .090 respectively for instance) and that there is a note on the face of the drawing stating this.
Now your left with dimensioning only those blends that don't fall within the 'standard' size... I don't see where using the sketches, or the curves representing the sketches and the associated dimensions will be of any benefit towards a casting/mach drawing. Dimension to the model. Very few radius dimensions will be difficult, and those could be handled easily enough. When the sketches were developed, it's very unlikely that the draftsman was even considered. So now the dimensions inherited from the sketches are essentially useless.
Clear as mud?

SS

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[Xwheelguy]

I'm just guessing again, but I think he might be trying to dimension radii from a non-standard point of view, like trying to dimension a radius from the top view, which is probably not typical for an edge blend unless the radius is created from a flat sketch in the XY plane (when looking at the top view).

Based on his descriptions, I have no idea of any CAD software that can do what he seems to be wanting to do. It's almost as if 3D annotation would serve his purposes better than putting all this effort into fudging the views in Drafting. It also sounds like the customer has no clue about making their drafting standards or requirements in line with what the software can and cannot do.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[cowski]

...trying to dimension radii from a non-standard point of view...

Another possibility is the taper was applied after the blend, which makes the edge geometry into an ellipse or intersection curve. That makes it a little more difficult to apply a radius dimension.

But I agree, without seeing the file we are all guessing.

 

[amatmay]

1)If you have done the drafting using master model consept then setting up a new reference set with the sketch and solid body (whose drafting u want to make), then replace the reference set in the drafting file,Make the sketch layer 'selectable' AND same layer visible in the required view.
2)If your drawing is not a mastermodel then just make the Layers 'selectable' and 'visible in view'
hope this will work!!