Dimensioning in Sketcher

[ptc-2741172]

Not to compare Pro/E with other programs I have used but I am finding difficulty getting used to this one. Why when I create geometry in sketcher no dimensions show up unless I create a second unwanted geometry and then click undo? Why does it automatically dimension it to a reference that I don't want? Why can't I figure out how to add a dimension? I click on normal (define a dimension) it asks for one selection, ok, nothing? I can use the drop down menu sketch, normal, reference it only asks for one selection, then nothing. I want to use this in the schools but I am not so sure it will work well.

[Kevin]

In my opinion you're going to drive yourself mad if you try to compare how things are done in one program versus another. Dimensions don't show for a sketched object until you finish the feature creation. If you are sketching a line pick your end points and select the middle mouse button to finish the feature and dimensions should show. The initial dimensions are weak dimensions so don't get hung up on the fact that dimensions are shown to references you don't want; you can change that. To add a dimension for the length of a line select the line put your cursor where you want the dimension and select the middle mosue button to create a strong dimension. If you try and create a dimension that conflicts with these you will get a dialog prompting you to resolve the problem. To dimension to a reference select the reference then the line (doesn't have to be in that order) then the middle mouse button. Using Sketch>Dimension>Normal will create a regular dimension. Selecting reference will create a reference dimension (dimension in parenthesis). Depending on the selection you make ProE may need another selection before it can create the dimension such as dimensioning a line to a reference. There are other selections needed for things like angular, radius, and diameter dimensions There is a tutorial and other resources you may want to look at under the Resource Center>Pro/Engineer Resource Center.

[mfischer]

Hi Frank, When you create a sketch in Pro/E, Sketcher shows you the dimension right away. Those are typically light gray dimensions. These are called week dimension and what Pro/E assigns. Everything in Pro/E is fully dimensioned. You can then assign you own dimensions if you want. These are called strong dimensions. You might check you toolbar to see if the dimensions are being displayed. Note: you do not have to finish creation of the feature to see the dimensions. Check out some of the basic tutorials on this page to assist you. There is one on sketcher. www.ptc.com/go/tryout Thanks, Mark

[KrisR]

Kevin is right....you will drive yourself "mad".

Pro creates dimensions on everything as soon as geometry is placed. As Mark stated, all geometries are dimensioned with "weak" dimensions that are light grey. You can long right click on them and make them "strong" dimensions which will define and constrain your design intent,

But even if dimensions are "strong", they does NOT mean that you cannot drag the geometry and change the dimensions. In order for the geometry not to change, you have to "lock" the dimensions. While in a sketch, you can go to "Sketch"->"Options" and checkmark for all user-defined dimensions to be locked. That way, they will not be able to be moved.

Pro is different from anything else out there....it takes getting accustomed to, and even then, you will miss features from other 3D programs you have used.

[AdamHaas]

Pro/E (Creo) can be setup so that modified dimensions automatically become locked. Our commercial customers typically set this option to YES, however, based on input from our academic university customers we have have left the option at the default NO setting.

If you would like to turn on this behavior, use the following config.pro option:

sketcher_lock_modified_dims yes

I hope this helps. Personally, I sometimes like this set to YES and other times I like it set to NO, it all depends on what I am doing and the type of features I am working with.

Regards,

Adam