grid lines

[Anonymous]

Dose inventor professional 2020 have the grid line?

if yes , kindly can you show me how to do them ?

[mcgyvr]

Inventor does not have a built in gridlines function..

Seems others have created workplanes in the 3d model and then brought them into the drawing and then added balloons (sketch symbol) to the end of each of those workplane lines.

There is an app to help automate that.. https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=5598923342182433135&appLang=en&os=Win64

Trial and paid version

https://apps.autodesk.com/INVNTOR/en/Detail/Index?id=8679646845906697765&appLang=en&os=Win64

[johnsonshiue]

Hi! Out of box, there isn't a command creating such grid lines in one shot. But, it is not too difficult to create those using Sketch Symbol workflow.

Many thanks!

[cadman777 · Accepted solution]

I found workplanes and workaxes to be a BAD IDEA. It creates extra overhead that you don't want.

The way I do it is create a Grid Line part (ipt) and make your base sketch/s on the elevation/s you want the grid lines, and then make your grid lines using sketch Lines. Then change the line type of all the lines to either centerline or phantomline. Then make a Symbol that can change the text and put that at the end of each line. Then save the file as your Grid Lines file. You can do this for both plan views and elevation views. Whatever you need. I've done this very successfully on some pretty big projects. One project had 75 structural and detail drawings. The 'details' were mostly on 2 sheets b/c they were repeats, so most of the drawings were one-off's.

Then, if you need to change the extension length of the grid lines or adjust the spacing, just open the Grid Line part and edit the sketches. If you want to reference those grid lines in a part file, then Derive the Grid Line part into that part file and add workpoints/axes so if the Derived file changes, the workpoints/axes will update w/the change.

In any structueral steel program the first thing you do is lay down your grids. So that's what I do in Inventor. The only thing missing is STRUCTURAL CONNECTIONS in the FrameGenerator and AUTOMATIC DETAILS in the idw file! If I was a coder, I would've done it already!

[Anonymous]

Thanks Cadman777 that was very helpful .

[cadman777]

Here's a very simple example of how you can do it.

This took me an hour to make.

The 3d model, underlying 3d sketch and drawing were simple and took only a few minutes.

I erred when saying you can use a Symbol in the part environment.

I also mistakenly thought you have to use Blocks instead in the part file.

But Blocks don't do you any good for labeling b/c there's no way to make the label changeable like w/Symbols.

So I just copy-and-paste the circle and text, then change the text.

Once you have one row or column of labels done, you can copy them all and reattach to the gridlines on the opposite side.

Anyway, that's how I've always done it b/c there was no way to do it automatically.
I guess that's another simple applet that the developers have lagged behind in adding to Inventor...Gridlines and Labels. Even when adding the smallest layout and structure to an existing building or work area you need gridlines. One has to wonder who FORGOT to add that to Inventor?? I can't tell you hoe many times over the years I've done this. Sometimes the project was of the type that I had to do it in AutoCAD of all things b/c Inventor didn't have the capability for documentation that structural work requires. How sad!

Incidentally, I've done this using Symbols in the drawing file, where the grid was made either like above or in the drawing file using a drawing Sketch. But I found that to be way too much work. The way I show in the attached dataset works best b/c the one sketch follows all your drawings through to the end.

[C_Down-NRS]

In your gridline.ipt did you just sketch the lines in a sketch?

I have been trying to do what you are saying but think I'm missing something...

I have attached my part

[cadman777]

Your sketch looks good.
It's similar to my example in this thread.

So if it's in your assembly, then you're good to go.

I'm not sure where your method is failing, so try this:

Download and open the zip file in 'Message 7'.

The assembly shows a part file w/the gridlines in it.

Open that part and you will see it is like yours.

Then open the drawing.

After you place a PlanView, you go to the model tree and expand the assembly part down to the gridline part.

Then you expand that part and RMB on the gridline sketch and pick 'Include, Visibility, Display Text'.

That gets your sketch to show up in the drawing view.

It will only show up in a drawing view that is perpendicular to the sketch plane (or at least that's how my older version works).

If in your grid part you add points at every grid intersection, and label them by their location, then you'll have a means to connect to your grid when working in the assembly, or if you Derive it into another part and need to reference the geometry for location purposes.  You can see that in my gridline file.

[C_Down-NRS]

It was just the turning on the sketch in the drawing which I was falling down, am running 2022 so slightly different menu...

Working great now thanks.

[rhasell]

Hi

All I can add,  I create an additional 3D sketch, I then project the 2D sketch to a 3D sketch, I find that the 3D sketches work much better in the detailing environment, they are always available for inclusion in the drawing views. (To explain better, I have two identical sketches of the grid, one 2D and one 3D sketch)

Depending on your environment, you don't even have to change the line type, as 3D sketches have their own layer, so this can be configured in the template.

I also use a prompted sketch symbol to place the grid line marks. (I have 4 default symbols with different insertion points)

For me, this is a stable and easily editable option, I find that editing text in the part environment is difficult.

[cadman777]

 I create an additional 3D sketch, I then project the 2D sketch to a 3D sketch, I find that the 3D sketches work much better in the detailing environment

Great idea! I never thought of that.

In the past I tried your method of using Symbols on Inventor drawings to mark the column lines.

The only thing is, whenever the drawing view changes or if it moves, the Symbols don't follow the lines they're connected to. So it always creates more work for me, rearranging symbols and all that.

Do you have the same problem?

If your Symbols don't disconnect from the lines they're attached to, how do you accomplish it?

Another thing about Symbols is, I could never figure out how to get the textbox to adjust to the text width.

I wanted to use the textbox to get the balloon to adjust size when the label width expands?

Have you figured that out?

And how do you get dimensions to attach to your symbol balloon on the opposite side of the connection point so the extension line doesn't cut through the text?

[rhasell]

As long as they snap to the lines, preferably the end of the line, they will move with the sketch and drawing view.

[rhasell]

I was going to send a drawing, but I am on 2022, I see you are still on 2010, so that won't work.

I made a quick video, I don't have screencast installed.

Apologies for the potato quality

[rhasell]

Hi

To answer the other questions:

I don't know how to automatically size the balloon with the text, most of my text entries are fairly common, but when needed, I will just make a new symbol with a larger balloon to suit.

I am not sure I understand your last question regarding the dimension.

[cadman777]

OK, thanx.

[cadman777]

Yes, they do.

But sometimes they disconnect, which means I have to place a new one, b/c the existing one won't reconnect.

Any ideas why that may be happening?

[C_Down-NRS]

Inventor is not a very good CAD system at all......that's my guess

[cadman777]

Nice video!

Yes, I see it works like that.

But sometimes my balloons disconnect, and I never figured out why.

Any ideas?

[cadman777]

LOL!

It's not nearly as good as I would like, but it's good enough...LOL!

[cadman777]

Last question:

I place dimensions between column lines and attach them to the balloon on the underlying sketch.

But with Symbols, the dimensions won't attach to the balloon, so they have to attach to the column lines, which means the dimension's extension line cuts through the balloon and the text.

How do you get the dimension to attach to the Symbol balloon?