How do people dimension to Silhouette Points in SW?

[bnemec]

We've been hacking it with lines and sketch points "attached" to the edge but if the model is changed and the line or point becomes detached it's easily missed and since the dimension is attached to the line/point it is not dangling so doesn't change color. We were used to automatic snap points on these edges that allowed dimensions to be easily placed.

How am I supposed to place this dimension without adding sketch elements on the drawing view?

[Glenn Schroeder]

I don't work with splines much, but can you put horizontal construction lines in the model sketch and make them tangent to the spline, show the sketch in the drawing view, dimension to it, then hide the sketch? (When you do that the dimensions may disappear; right-click on the sketch in the tree and select "Show dimensions" if it does.)

[Tom G]

Could you define reference planes by parallel and tangent, and dimension to those?

[bnemec]

Thank you for the suggestions, however if I understand correctly we're fixing the problem in the model instead of the drawing. This causes some problems:
- the sketch planes are seldom in plane with drawing views and often the geometry in the finished part does not follow the sketch.
- I seldom use splines in my sketches, all lines and arcs, the non-primitive surfaces are results of drafting and fillets in many cases. Other times the faces are results of lofts or sweeps. Maybe I shouldn't have said spline, I'm not sure what to call it other than the projection edge of a non-primitive surface?
- Sometimes other people work on the drawing than who did the model and for them to go back into the model and start adding a bunch of planes and sketches sometimes lead to a mess.
- These parts are often dimensioned to in the drawings of upper level assemblies where the projection is different than it would be in the piece part drawing so now we have more planes and sketches that we hope happen to be at the correct angle for the drawing view. Now with PDM we often wouldn't be able to edit the part when doing an upper level drawing as the part is likely in a Released state.

[SPerman]

I was confused because I thought you were talking about this type of spline.

[KennyG]

How am I supposed to place this dimension without adding sketch elements on the drawing view?

You turn on your IntelliSketch "Silhouette Point" and select that point when placing your Dimension Between.

Oh wait, wrong app

[bnemec]

You turn on your IntelliSketch "Silhouette Point" and select that point when placing your Dimension Between.

Oh wait, wrong app

As I read this I cussed myself for not finding how to do such an obvious task, especially since I'd already seen that because I remember the terminology.

Then I read on and cussed you for teasing me as I realized I remembered the term from Solid Edge where dimensioning to a SILHOUETTE POINT was a simple part of daily life. I thank you for explaining perfectly the process I am trying to do. It's just that the process is only available in the CAD system we mistakenly left.

Why does it feel like I'm dimensioning to a 3D object when I'm in a Solidworks drawing? In solid edge the elements to which the annotations connected to were on one plane, already projected.

[bnemec]

I was confused because I thought you were talking about this type of spline.

image.png

I am the one who is confused. I thought what you have pictured are called involutes.

[SPerman]

AFAIK, involute is the geometry that describes the shape of the spline.

https://en.wikipedia.org/wiki/Involute

[SPerman]

Can you dimension to the sketch points that describe the spline?

[matt]

Often features like that are made with sketches that have some construction geometry. Centerline connected to spline points. Sometimes you can dimension to actual feature sketches.

If there are no appropriate feature sketches, then, yes, your method with the sketch elements is the method I use.

You have to know what's the purpose of the dimension. Is it a real driving dim, inspection, reference... Etc.

[Cadmonkeychris]

I don't work with splines much, but can you put horizontal construction lines in the model sketch and make them tangent to the spline, show the sketch in the drawing view, dimension to it, then hide the sketch? (When you do that the dimensions may disappear; right-click on the sketch in the tree and select "Show dimensions" if it does.)

Another way to hide the construction lines is to stick them on a dedicated layer and then hide / unhide the layer as required. Dims will remain visible if not on that layer.

[AlexLachance]

I don't work with this and use pretty much the same method as you, but if I were to work with these and wanted to "avoid" the issue you described, I'd try having feature sketches dimension shown. Pretty sure the change done at the part level never "loses" it's reference unlike the sketch point would in the drawing. When they are indeed lost in the feature sketch level, it is generally when the geometry is being modified. In those cases, generally speaking of course, the draftsman/engineer/technician then reattaches the elements in the feature sketch, so that the errors in the sketches disappear.

[bnemec]

I shouldn't have used the "spline" word in my first post, that's my mistake. There's no splines in any sketch on this part. The sketch for the revolve feature that makes the base of this solid is normal to the drawing view. In other cases the finished geometry doesn't match the base sketches after drafts and radii are applied.

It seems like dimensioning to the sketches in the model is the most popular response, but I struggle to comprehend that. I try to model for a robust and stable model, I'm not thinking, "How can I sketch this so that I can dimension the part in the drawing?"

[dave.laban]

Dimension in the model and use Import Model Items in the drawing always works for me, especially for the sorts of dimensions that would be flaky when applied in the drawing environment.

[bnemec]

Dimension in the model and use Import Model Items in the drawing always works for me, especially for the sorts of dimensions that would be flaky when applied in the drawing environment.

What kind of stuff are you modeling? I must be doing it all wrong! The sketches I make in a model are 90% useless in a drawing. Didn't we move away from making 2D drawings and move to making 3D models and placing dimensions to geometry a couple decades ago?

[AlexLachance]

What kind of stuff are you modeling? I must be doing it all wrong! The sketches I make in a model are 90% useless in a drawing. Didn't we move away from making 2D drawings and move to making 3D models and placing dimensions to geometry a couple decades ago?

I'm guessing dave creates the required dimensions through a 3D sketch or simply by creating reference dimensions, and then he has these dimensions uploaded from the model by using import model items.

I think you're seeing this the wrong way. It's basically the same as doing the dimensions inside the drawing, except you do it on your model instead and then import them, because the model tends to fail less then 2D generated geometry in a drawing.

[Glenn Schroeder]

We've been hacking it with lines and sketch points "attached" to the edge but if the model is changed and the line or point becomes detached it's easily missed and since the dimension is attached to the line/point it is not dangling so doesn't change color. We were used to automatic snap points on these edges that allowed dimensions to be easily placed.

How am I supposed to place this dimension without adding sketch elements on the drawing view?

image.png

Can you post that model (or one similar if it's proprietary)? I'd like to try something.

[bnemec]

I'm guessing dave creates the required dimensions through a 3D sketch or simply by creating reference dimensions, and then he has these dimensions uploaded from the model by using import model items.

I think you're seeing this the wrong way. It's basically the same as doing the dimensions inside the drawing, except you do it on your model instead and then import them, because the model tends to fail less then 2D generated geometry in a drawing.

Ok! Thank you for explaining that, you're spot on, I seeing it wrong. The training of "look how cool SW is" showed using the sketches that made the part used in the drawing so just as you mentioned, that's how I was thinking of it. I never thought of adding sketches at the end of the feature tree after the model is done for the sole purpose of using them in the drawing.

So many people are doing the drawing dimensions and attached annotations/callouts in the model so the drawing works better?

[bnemec]

Can you post that model (or one similar if it's proprietary)? I'd like to try something.

Technically, I shouldn't have posted the screen shot in public domain. I was throwing together a generic model earlier that replicates the behavior but Solidworks "had to close." Of course doing scratch work I hadn't saved yet, then I had to go to a meeting and after that I didn't start it again. But since you asked I'll try to make a model and drawing to share.

[matt]

I think you have to think about how you're going to use the dimension. Is it only reference? Do you really need 3 or 4 places on that dimension? Do you have a fixture or some special technique/tool to measure it? If it's difficult to create the dimension in CAD, it's probably also difficult to physically measure it. If it's just for CNC reference, that's a different story.

Dimensioning splines is a waste of time 98% of the time. Let the CNC do it's job, and make sure you are using the correct machining parameters, using good cutters, the machine is well maintained, the work is fixtured properly, and it will be ok. Same with 3d print. Make sure you're using a machine with the kind of tolerances you need.

[AlexLachance]

Ok! Thank you for explaining that, you're spot on, I seeing it wrong. The training of "look how cool SW is" showed using the sketches that made the part used in the drawing so just as you mentioned, that's how I was thinking of it. I never thought of adding sketches at the end of the feature tree after the model is done for the sole purpose of using them in the drawing.

So many people are doing the drawing dimensions and attached annotations/callouts in the model so the drawing works better?

I wouldn't say many, but when your line of work causes this kind of behavior, I'd guess that's how you'd try to "work around" the undesired behavior of lost relations that aren't noticeable. Having them at the part level gives "errors" while in the drawings they aren't noticeable errors.

For instance, we work somewhat like that, but not exactly. We create dimensions at the part level so that we can use them in properties.

[AlexLachance]

Just to clarify a bit more:

you do it on your model instead and then import them, because the model tends to fail less then 2D generated geometry in a drawing.

The geometry inside the drawing is "converted", so when you're seeing a front view, rather then show a radius, in a drawing it might be a "spline" or what not, so doing the dimensions inside the model, rather then inside the drawing, to then upload them inside the drawing, will give a better "result" because the dimensions inside the model are attached to true geometry whereas the dimensions inside the drawing are attached to converted geometry that will "reconvert" itself everytime.

Hopefully I'm being clear lol

[bnemec]

I think you have to think about how you're going to use the dimension. Is it only reference? Do you really need 3 or 4 places on that dimension? Do you have a fixture or some special technique/tool to measure it? If it's difficult to create the dimension in CAD, it's probably also difficult to physically measure it. If it's just for CNC reference, that's a different story.

Dimensioning splines is a waste of time 98% of the time. Let the CNC do it's job, and make sure you are using the correct machining parameters, using good cutters, the machine is well maintained, the work is fixtured properly, and it will be ok. Same with 3d print. Make sure you're using a machine with the kind of tolerances you need.

Measured with calipers for small parts. Often on small parts where the tooling is based on model we're showing overall dims and those can be ref. If the silhouette points (max/min distance to tangent of projected edge) is important we try to use GD&T to better define it. Yes the model contains the geometry but at the end of the day, when it comes to accepting or rejecting purchased parts the drawing is the legal controlling document.

The bulk of our prints that need these dims are top level and measured with tape measure to upholstered foam. Regardless of how they are measured they need to be on the print. If they are on the print, in my opinion they should be attached to model geometry if at all possible.

Edit: I should maybe add that these dimensions are not something new we are adding to our process. We are trying to maintain functionality that we had before. If these dimensions were not needed we wouldn't have been putting them on the drawings all these years.

[bnemec]

I wouldn't say many, but when your line of work causes this kind of behavior, I'd guess that's how you'd try to "work around" the undesired behavior of lost relations that aren't noticeable. Having them at the part level gives "errors" while in the drawings they aren't noticeable errors.

For instance, we work somewhat like that, but not exactly. We create dimensions at the part level so that we can use them in properties.
image.png

That is exactly what we're trying to do.

[Glenn Schroeder]

Technically, I shouldn't have posted the screen shot in public domain. I was throwing together a generic model earlier that replicates the behavior but Solidworks "had to close." Of course doing scratch work I hadn't saved yet, then I had to go to a meeting and after that I didn't start it again. But since you asked I'll try to make a model and drawing to share.

Maybe there's something going on there that I can't follow from the screenshot, but if those are arcs instead of splines you should be able to dimension to their outer edges just by holding down the Shift key and clicking on them with the Smart Dimension tool active.

image.png (11.82 KiB) Viewed 5371 times

Again, I suspect there's something else going on, which is why I asked for a model.

[bnemec]

Maybe there's something going on there that I can't follow from the screenshot, but if those are arcs instead of splines you should be able to dimension to their outer edges just by holding down the Shift key and clicking on them with the Smart Dimension tool active.


image.png


Again, I suspect there's something else going on, which is why I asked for a model.

Thanks Glenn, I forget the shift key when placing dimensions I'm still new to Solidworks. It works when the projected edge is still an arc which happens to be the case the screen shot in first post but most of the time the projected edges of the molded foam models in top level drawings are not arcs. Most of them that I'm looking at there are so many short edges that people just grab the endpoint of one and call it close enough, and it usually is as long as the silhouette of the part is segmented enough near the crest.

I get a lot of this when holding shift down and selecting a projected silhouette.

[Glenn Schroeder]

Thanks Glenn, I forget the shift key when placing dimensions I'm still new to Solidworks. It works when the projected edge is still an arc which happens to be the case the screen shot in first post but most of the time the projected edges of the molded foam models in top level drawings are not arcs. Most of them that I'm looking at there are so many short edges that people just grab the endpoint of one and call it close enough, and it usually is as long as the silhouette of the part is segmented enough near the crest.

I get a lot of this when holding shift down and selecting a projected silhouette.
image.png

I am painfully well acquainted with that message. I usually resort to placing sketch elements in the drawing, use relations to lock them in place relative to the model, dimension to them, and then move the sketch elements to a Layer that's turned off.

However, all too often in those situations it also won't let me apply a relation. In that case I usually add sketch elements in the model, show the sketch in the drawing, dimension to it, then hide the sketch.

Of course when I do that the dimension is often hidden also, so I have to find the sketch in the tree again, right-click on it, and select "Show dimensions". I'm still trying to figure out the logic behind the software automatically hiding a dimension I just placed. I've even had cases where I'd insert two dimensions between the sketch and mode l edges, hide it, and only one of the dimensions would be hidden. I would really like someone to explain that one to me with a straight face.

[SPerman]

I've had the same experience and frustration with showing sketch dimensions in the drawing.

[dave.laban]

What kind of stuff are you modeling? I must be doing it all wrong! The sketches I make in a model are 90% useless in a drawing. Didn't we move away from making 2D drawings and move to making 3D models and placing dimensions to geometry a couple decades ago?

I've done a combination of oil/gas drilling equipment (typically Ø5 x 48" intricately machined single pieces of steel), battery assembly lines (thousands of small pieces per assembly, can see some overall product images here http://www.tbseng.co.uk/cos-machines ) and specialist electronics housings ( https://www.allenvanguard.com/3xxx-ecm/ but all the good stuff is on the inside). I can see the limitations of Import Model Items when it comes to complex organic shapes but for anything where orthogonal views are enough to convey the part then it's a huge time saver (assuming you can rewire your brain to produce the drawings in a compatible manner).

I'm guessing dave creates the required dimensions through a 3D sketch or simply by creating reference dimensions, and then he has these dimensions uploaded from the model by using import model items.

Never a 3D sketch at the end, occasionally reference dimensions added within the production sketch, normally everything straight from the sketch geometry used to create the part.

Only time I'm regularly creating dimensions in the drawing environment is if I've got multiple features dimensioned using Ordinate Dimensions that all share a common Datum - because you can't sensibly merge them in the drawing view I find it easier to quickly recreate the 2 or 3 Ordinate Dimensions in to one so I then get all the auto-jogging for free.

[jcapriotti]

Does any 3d cad do this well? I remember using NX years ago for curvy medical stuff and we needed to place overall dimensions. I had to extract the edge as a spline, then "convert to arcs" the spline so I could place the dimension. It lost the associativity to the model so you had to watch updates.

[bnemec]

Does any 3d cad do this well? I remember using NX years ago for curvy medical stuff and we needed to place overall dimensions. I had to extract the edge as a spline, then "convert to arcs" the spline so I could place the dimension. It lost the associativity to the model so you had to watch updates.

@KennyG do you have a video or link handy that shows how effortlessly dimensions can be placed to silhouette points in Solid Edge drafting?

[the_h4mmer]

For these kinds of issues, I have a few solutions:

1. Expand the drawing view, expand the design feature tree, find the appropriate sketch, unhide, add dimensions, and then rehide the sketch. That's all assuming that the feature I need to dimension can be pulled directly from a model sketch, and would be the best means of accomplishing this as the dimension should update correctly if/when the feature is updated (problems ensue of course when sketch entities are removed, but if that's happening I'd argue it mayy have been too early to start on the drawing).

2. In the model, add planes relative to the feature to be dimensioned, that are perpendicular to the drawing view where the dimensioning is needed. In the drawing, expand drawing view, feature tree, unhide planes, add dimensions, and hide planes.

3. If neither of the two above work, I will add sketches at the end of the model feature tree to using for dimensioning.

4. Failing all else, I add sketch geometry to the drawing that is placed on a dedicated hidden drawing layer.