transitioning from a straight line to a fillet to a straight line

[Mike Gera]

In a part sketch, what is the most efficient workflow for transitioning from a straight line to a fillet and then back to a straight line?

Currently, for example, I'll draw a 90-degree hard corner, then as a secondary operation, add a sketch fillet.

I'm pretty sure there's a way to add the sketch fillet "on the fly".

Thanks for any replies.

[Frederick_Law]

[DanPihlaja]

Well, there is this:

There are 2 ways to draw a line in Sketcher.
Click and Drag
Click, release, move the mouse, click release.

If you use the 2nd method, then a 2nd line will be formed with its attachment point at the end point of the last line.

When you are at this stage, if you hit the "A" key, it will switch to drawing an arc. Once you place the arc, it will automatically transition to drawing a line again. if you hit the "A" key again, it will switch again to drawing an arc.

Is this what you mean?

[Glenn Schroeder]

For me it depends on the situation. If I just need one then I move my cursor back to the end of the straight line, like shown in the video @Frederick_Law posted. If I want multiple fillets, and especially if I want them equal, I use the sketch fillet tool.

[Mike Gera]

Thanks, Frederick.

This works, but it does require that I then go back and add two "tangency relations. Is there a way to avoid having to do that?

[gupta9665]

This works, but it does require that I then go back and add two "tangency relations. Is there a way to avoid having to do that?

When you add the arc, SW should automatically add the tangent relation. It does for me using both options i.e. on pressing A to start the arc OR dragging the cursor back and start the arc.

[AlexLachance]

Thanks, Frederick.

This works, but it does require that I then go back and add two "tangency relations. Is there a way to avoid having to do that?

The tangency relations are supposed to add themselves automatically. Not the case on your end..?

[Mike Gera]

The tangency relations are supposed to add themselves automatically. Not the case on your end..?

Not happening on my end.

[gupta9665]

Not happening on my end.

I know it is stupid to ask but check if "automatic relation" is set to on. If all settings are good then knock on your VAR door.

[DanPihlaja]

Thanks, Frederick.

This works, but it does require that I then go back and add two "tangency relations. Is there a way to avoid having to do that?

It depends on where you place your cursor when you hit the "A" key. It is intuitive about where the cursor is.

[Mike Gera]

I've now gotten it to the point where I need to add one tangency.

[DLZ_SWX_User]

For me it depends on the situation. If I just need one then I move my cursor back to the end of the straight line, like shown in the video @Frederick_Law posted. If I want multiple fillets, and especially if I want them equal, I use the sketch fillet tool.

I am of the same mind as Glenn. It all depends on what I want to achieve or how I want to control features.

I've now gotten it to the point where I need to add one tangency.

This is all that I have been able to achieve also.

[Glenn Schroeder]

The arc is automatically tangent to the first line, but I'm able to get the other one tangent also. If you can't I suspect one of the options at Tools > Options > System Options > Sketch > Relations/Snaps isn't checked.

[Mike Gera]

The arc is automatically tangent to the first line, but I'm able to get the other one tangent also. If you can't I suspect one of the options at Tools > Options > System Options > Sketch > Relations/Snaps isn't checked.

image.png

Hi Glen,

This is how they're set:

[Glenn Schroeder]

Hi Glen,

This is how they're set:

Then I can't imagine why you can't get the second line tangent.

Something just occurred to me. After clicking to place the arc, and moving your cursor to start a line from its endpoint, you will only get the option to make this line tangent to the arc in its present location. If your cursor isn't close to tangent with the arc then you won't get the option.

If you don't, applying the tangent relation later is so simple that it's not worth spending much time worrying about (at least in my opinion). All you have to do is click on the point where the line and arc join, then click on the Tangent icon. Of course you can achieve the same thing by Ctrl+selecting the line and the arc, but it's not necessary as long as the end point isn't shared by a third sketch entity.

[Mike Gera]

Then I can't imagine why you can't get the second line tangent.

Something just occurred to me. After clicking to place the arc, and moving your cursor to start a line from its endpoint, you will only get the option to make this line tangent to the arc in its present location. If your cursor isn't close to tangent with the arc then you won't get the option.

If you don't, applying the tangent relation later is so simple that it's not worth spending much time worrying about (at least in my opinion). All you have to do is click on the point where the line and arc join, then click on the Tangent icon. Of course you can achieve the same thing by Ctrl+selecting the line and the arc, but it's not necessary as long as the end point isn't shared by a third sketch entity.

image.png

How exactly are you transitioning from placing the 2nd (and final) arc point back to a straight line?

Thanks.

[Mike Gera]

OK, I now see what the problem is and where the confusion lies. I'm able to infer the 2nd tangency relation, but not necessarily at the desired 90 degrees. I'm basically trading the tangency for the perpendicularity.

[Mike Gera]

Does SolidWorks have an ORTHO mode?

[Glenn Schroeder]

OK, I now see what the problem is and where the confusion lies. I'm able to infer the 2nd tangency relation, but not necessarily at the desired 90 degrees. I'm basically trading the tangency for the perpendicularity.

That's correct.

Does SolidWorks have an ORTHO mode?

I don't know. Can you please explain what that is for the slower members of the class (like me)?

[DanPihlaja]

Does SolidWorks have an ORTHO mode?

Sort of. You can kind of get an ortho mode by playing with these settings:

You then have to view the grid using this:

And define the grid here:

[Glenn Schroeder]

OK, I now see what the problem is and where the confusion lies. I'm able to infer the 2nd tangency relation, but not necessarily at the desired 90 degrees. I'm basically trading the tangency for the perpendicularity.

I just checked. You can get both perpendicular and tangent (assuming the first line was vertical or horizontal, at least). When placing the arc, if you will click to finish it when you see the blue horizontal and vertical dotted lines then you can place the second line with the relations you want.

image.png (10.76 KiB) Viewed 4293 times

image.png (9.79 KiB) Viewed 4293 times

[Mike Gera]

That's correct.

I don't know. Can you please explain what that is for the slower members of the class (like me)?

Imagine a world where uppey/downey and leftie/righie was all you had.

[Frederick_Law]

Or sketch with corners and add fillets after.
https://help.solidworks.com/2021/englis ... illets.htm

[Mike Gera]

I just checked. You can get both perpendicular and tangent (assuming the first line was vertical or horizontal, at least). When placing the arc, if you will click to finish it when you see the blue horizontal and vertical dotted lines then you can place the second line with the relations you want.


image.png

image.png

No matter what I do, I don't see the horizontal and vertical ghost lines. What version os SW are you running?

[DanPihlaja]

No matter what I do, I don't see the horizontal and vertical ghost lines. What version os SW are you running?

You might need to have this checked:

[DLZ_SWX_User]

Thanks @Glenn Schroeder ! This looks like it'll be a benefit to my sketching in more ways than one!

You might need to have this checked:
image.png

This is what I normally would do.

Or sketch with corners and add fillets after.
https://help.solidworks.com/2021/englis ... illets.htm

[SPerman]

No matter what I do, I don't see the horizontal and vertical ghost lines. What version os SW are you running?

I'm on 2022 SP5 / W11 like you. The only time I see the ghost lines is if there is a dimension referencing the line (and "keep constrained corners" is checked.)

From the SW help:

Keep constrained corners: Maintains the virtual intersection point if the vertex has dimensions or relations. When cleared, and if the vertex has dimensions or relations, you are asked if you want to delete those geometric relations when the fillet is created.

[Frederick_Law]

This is what I normally would do.

This would be faster and easier to control. Usually.
Another is fillet feature which should be used before sketch fillet.

[Glenn Schroeder]

No matter what I do, I don't see the horizontal and vertical ghost lines. What version os SW are you running?

SW2023 sp 3.0

[john@layketool.com]

The tangency relations are supposed to add themselves automatically. Not the case on your end..?

It seems that the first transition from the line to an arc will get the tangency relation added but the transition from the arc to the 2nd line will not add the tangency relation unless you position the line to be tangent. Would be like making a slot and unless you stop the point of the arc end at the exact point of tangency and then add the line, it will not be tangent.

[Krzysztof Szpakowski]

It looks like you have disabled automatic relations in menu TOOLS - SKETCH SETTINGS - AUTOMATIC RELATIONS