Problem with custom drawing border

Hi Guys,

I have just gone back to training myself to use SolidWorks and run head long into a problem whilst creating a new custom 2D drafting border.

I began with the stock SolidWorks title block and modified it to be my own. I found serveral hidden notes that I can neither delete, move, or do anything with at all - see screen image.

Can someone please tell me how to manipulate them?

Thanks for your help.

Regards,

Dave

The boxes you see are text fields. The ones that just come up and say font size are blank so when you double click on the title block you can enter the data. If they have something like $PRPSHEET or $PRP that means they are a defined property or sheet property that will autofill if the data is available. For instance "Company Name" if filled out in your SW info will appear.

If you want areas to auto fill you do this in the "Edit Sheet Format" option when you right click on the Sheet Format. You will notice in the Title area it will say $PRPSHEET:{Description}. This field will auto-fill with the description(part name in most cases).

Are you looking to place text boxes that the user can enter data into or are you looking to create sheet properties that auto-fill based on info in the drawing/assembly?

Hi Matt,

I am aware of all you have outlined above, and in truth I have not yet decided whether to automate some of the title block text, or to apply it manually. Probably the latter, although I can appreciate the benefits of automation.

What I wanted to do was remove these text boxes altogether, possibly re-creating them at a later date, should I decide automation is the best way after all.

The image I showed is in "edit sheet format" and actually one step deeper into "edit title block," which is where these pesky hidden text boxes appear. No matter what I do I cannot re-position or delete them.

I guess an ideal situation for me would be for the title block to work in a similar way to an AutoCAD title block with hidden attributes. Attedit bringing up a pre-determined list that the user just fills in, job done.

Regards,

Dave

To create them you can go to Edit Sheet Format and add notes just as you would to the drawing from the annotations tab(leaving them blank), then go to Define Title Block and select the ones you want to become enter-able text boxes. When you are in Edit Sheet Format, they are there even though they really arent visible like in Define Title Block. You can select them, move them, edit their font and size or delete them here. This is also where you would Link them to properties. These properties could be standard ones that get filled out form File>Properties in each part file, or custom ones that you have created.

Let me know if that answered it for you. If not i can add more info/screen shots to help.

I should also note any info that you need in the title block or in BOM columns can be filled in or added as custom properties to part or assembly template files. I have been trying to get this implemented here because i make all the drawing files for a few users so if i could send out part and assembly template files and tell them what to fill out it would be easy for me to use SW scheduler and have drawings created over night Here are some screen shots of a custom property i added in the assembly, a text box added in edit sheet format that i linked to this custom property. There is an evaluated column because you can have numerical values, things like mass properties, time/date stamps, Yes/No drop boxes(say the property has to do with checking the design you could have a text box property for Checked by where they fill in their name and a property for them to check yes/no and then a date stamp. So 3 things get filled in by the user here and it would appear on the title block.

Sorry Matt,

But I must be missing something - I still cannot delete those notes. Do you mind if I send you my border for you to have a look at. If you can delete them, perhaps you can tell me exactly how you did it.

Thank you for your help.

Regards,

Dave

MDLtd_a2.zip

Sorry dave, im using 09 at work and it told me it was a future version.

When you open your drawing sheet and expand it in the feature tree(sheet 1 unless you have renamed it) right click on "Sheet Format1" and select "Edit Sheet Format". When you do this you will be able to select the sketch lines that make up your title block(just as a point of reference, not that you have to edit them). The text boxes are there but they arent visible until you click on them. Ive added notes to each image. See if this works for you.

Hi Matt,

Thanks, I've got it now It beggars belief that the user has to be in a mode where they cannot see the note boxes to be able to move and delete them. I have to say that this is a d*mn stupid way of working From my admittedly short use of SolidWork's it seems to be typical of the author(s) muddled way of thinking and doing things. I am surprised that so many people really like this program????

Thanks for your help, you have allowed me to move forward at last. Have a good weekend.

Regards,

Dave

No problem dave. I believe its setup this way so that the normal user cant accidentally go in and muck things up. When you are creating a custom title block you would likely be placing all your own blocks and this method of editing isnt really needed. For all i know there may be an option in the View menu that allows you to see them. Ive never been too worried about it because its a one time deal for me. I dont make title blocks except at the start of a large project.