How do I hide these lines

[Ömür Tokman]

Hi Guys
My first question on this forum and I am very excited.

How do I hide these lines.
the blue one is the flat line and it should be visible.
I have to hide the other lines one by one.
there is probably an easy way but I can't find it.
Thank you in advance for your help.

2021-04-16_14-38-04.png

[AlexLachance]

Most likely axises/sketch elements from patterns.

In your case, it looks like it's the bend line, so hide the bend line sketch inside the part.

[Ömür Tokman]

Thanks Alex,
yes they are twist lines but I can't understand why they appear. If it's something you approve, the lines in each part should be visible. But lines of random pieces are visible (not every piece), and the only way I can find so far is to hide each line individually.

[AlexLachance]

Thanks Alex,
yes they are twist lines but I can't understand why they appear. If it's something you approve, the lines in each part should be visible. But lines of random pieces are visible (not every piece), and the only way I can find so far is to hide each line individually.

If you recreate the view, do they still appear? They most likely appeared upon creation and need to be removed manually afterwards, so if you recreate the view you should be good.

If recreating the view is not an option, then perhaps using the Sketch filter in order to select only thes.
http://help.solidworks.com/2016/english ... ection.htm

image.png

[Ömür Tokman]

The lines are hidden in each part, the lines are hidden in the assembly, but they are still there in the drawing.
Filters cannot detect these lines.

[AlexLachance]

They are hidden inside your assembly because you have everything set to hidden Omur, the eye is "blacked out" meaning it's hidding all.

The filter I speak of is not that. The filter I speak of is a toolbar you can activate by pressing F5, and then you have a multitude of selection filters you can use.

[Ömür Tokman]

Isn't it the filters at the bottom of the first picture? I open it with F5.

[AlexLachance]

Isn't it the filters at the bottom of the first picture? I open it with F5.

Yes, sorry I had not seen that in the first picture, I thought that you thought I were refering to the hide/show filters from the eye, my apologies!

Would you like me to do a Teams session real quick with you and see if I can be of help?

[Ömür Tokman]

You don't have to apologize, Mate, actually I'm sorry for not clearly stating in the picture.
I'm not available for Teams right now. I have to send the drawings I have to the production department first.
Thank you very much for your kind consideration.

[AlexLachance]

You don't have to apologize, Mate, actually I'm sorry for not clearly stating in the picture.
I'm not available for Teams right now. I have to send the drawings I have to the production department first.
Thank you very much for your kind consideration.

Anytime Omur, if you ever change decision you can send me a private message. Have a great weekend.

[Ömür Tokman]

Thanks a lot Bro.

[jcapriotti]

Hi Guys
My first question on this forum and I am very excited.

How do I hide these lines.
the blue one is the flat line and it should be visible.
I have to hide the other lines one by one.
there is probably an easy way but I can't find it.
Thank you in advance for your help.
2021-04-16_14-38-04.png

Ömür, there are two ways to hide these sketches in the original part files. I think most people tend to use "Hide types (eye icon) and un-clicking "View Sketches". This just toggles them off globally in the part. The other way is in the feature tree for each sketch individually. This is the one you want as the Hide Types is more of a global override and, in my opinion, a temporary tool. Hiding the sketches in the tree is the correct way otherwise the sketches show in the assembly unless you toggle that Hide Types options again in the assembly.

When you create a drawing view, it picks up the sketch visibility status from the feature tree of the part. After view creation, the sketch visibility status is now independent of the part. So hiding in the part tree makes no difference except for new drawing views. For the existing view your have to hide the sketches one at a time.

Bottom line, for your models, as a last step when the design is done, make sure all sketches, planes, axis, etc are hidden in the feature manager tree.

image.png

[Glenn Schroeder]

Hi Guys
My first question on this forum and I am very excited.

How do I hide these lines.
the blue one is the flat line and it should be visible.
I have to hide the other lines one by one.
there is probably an easy way but I can't find it.
Thank you in advance for your help.
2021-04-16_14-38-04.png

Ömür, there are two ways to hide these sketches in the original part files. I think most people tend to use "Hide types (eye icon) and un-clicking "View Sketches". This just toggles them off globally in the part. The other way is in the feature tree for each sketch individually. This is the one you want as the Hide Types is more of a global override and, in my opinion, a temporary tool. Hiding the sketches in the tree is the correct way otherwise the sketches show in the assembly unless you toggle that Hide Types options again in the assembly.

When you create a drawing view, it picks up the sketch visibility status from the feature tree of the part. After view creation, the sketch visibility status is now independent of the part. So hiding in the part tree makes no difference except for new drawing views. For the existing view your have to hide the sketches one at a time.

Bottom line, for your models, as a last step when the design is done, make sure all sketches, planes, axis, etc are hidden in the feature manager tree.

I agree. The only time I ever click on the eyeball icon to hide everything is when I open a file someone has posted here (or on the old forum) and it has planes and sketches showing all over the place. I never use it working with my own files.

[Ömür Tokman]

Hi Guys
My first question on this forum and I am very excited.

How do I hide these lines.
the blue one is the flat line and it should be visible.
I have to hide the other lines one by one.
there is probably an easy way but I can't find it.
Thank you in advance for your help.
2021-04-16_14-38-04.png

Ömür, there are two ways to hide these sketches in the original part files. I think most people tend to use "Hide types (eye icon) and un-clicking "View Sketches". This just toggles them off globally in the part. The other way is in the feature tree for each sketch individually. This is the one you want as the Hide Types is more of a global override and, in my opinion, a temporary tool. Hiding the sketches in the tree is the correct way otherwise the sketches show in the assembly unless you toggle that Hide Types options again in the assembly.

When you create a drawing view, it picks up the sketch visibility status from the feature tree of the part. After view creation, the sketch visibility status is now independent of the part. So hiding in the part tree makes no difference except for new drawing views. For the existing view your have to hide the sketches one at a time.

Bottom line, for your models, as a last step when the design is done, make sure all sketches, planes, axis, etc are hidden in the feature manager tree.

image.png

Both have the same features but prt1 is visible and prt2 is not.

[AlexLachance]

Omur, please look in the sheet metal folder(düz-çogaltma) where the unbent version is. There are sketches in there that are not supressed and sometimes they flicker and start showing up. Maybe that's one of those?

Also, are you using configurations or display states? If your assembly contains the part in a different display state and/or configuration, then that would explain why you don't see the issue inside the part.

[jcapriotti]

Check under the sheet metal flat pattern folder. Even though its suppressed, the "bend lines" sketch often isn't. If it was visible at the time of drawing view creation, it may still be on in the view tree.

image.png

[DanPihlaja]

Hi Guys
My first question on this forum and I am very excited.

How do I hide these lines.
the blue one is the flat line and it should be visible.
I have to hide the other lines one by one.
there is probably an easy way but I can't find it.
Thank you in advance for your help.
2021-04-16_14-38-04.png

Try turning on this option:

image.png

[Ömür Tokman]

Check under the sheet metal flat pattern folder. Even though its suppressed, the "bend lines" sketch often isn't. If it was visible at the time of drawing view creation, it may still be on in the view tree.

image.png

Bend lines are hidden for all parts, I don't use config.

[Ömür Tokman]

2021-04-16_14-38-04.png

Try turning on this option:

image.png

it was already open

[jcapriotti]

Check under the sheet metal flat pattern folder. Even though its suppressed, the "bend lines" sketch often isn't. If it was visible at the time of drawing view creation, it may still be on in the view tree.

image.png

Bend lines are hidden for all parts, I don't use config.

In the drawing view, expand down to the same folder for the part showing the lines.

[SPerman]

Have you tried turning off annotations?

[Ömür Tokman]

Check under the sheet metal flat pattern folder. Even though its suppressed, the "bend lines" sketch often isn't. If it was visible at the time of drawing view creation, it may still be on in the view tree.

image.png

Bend lines are hidden for all parts, I don't use config.

In the drawing view, expand down to the same folder for the part showing the lines.

Yeah that is right,
Well, do you know what is the reason for this? or what is the way to prevent it?

2021-04-16_18-10-23.png

normally I click the line and hide it.

2021-04-16_18-13-32.png

[jcapriotti]

Yeah that is right,
Well, do you know what is the reason for this? or what is the way to prevent it?
2021-04-16_18-10-23.png

normally I click the line and hide it.

2021-04-16_18-13-32.png

When the view was created, the sketch must've been on in the model tree but now no longer is. On drawing view creation, the sketch status are copied to the drawing view's version of the tree.

[Ömür Tokman]

Okay thank you Jcap. As far as I understand, we have to create a technical drawing after completing all the deficiencies. this makes sense, I am reviewing each part file one by one. Thank you again.