Solidworks 2005 can't change dimensions

[randyf1965]

I create a new part and after making a large rectangle with a rectangular cut in it. I can't change any dimension. I get the properties windows to come up but the box where I could change the dimension is greyed out.

Is there something I changed?

[JerryFlyGuy]

have you right clicked the feature in the tree and selected edit sketch?

Got a screen snap of it??

Jerry

[randyf1965]

Sorry this is an imported part.

[JerryFlyGuy]

thats your problem then, your not going to be able to change dimensions on an imported part, as there are no driving sketch's to change.

either you re-draw it, or live with it the way it is.

Jerry

[randyf1965]

Doh..... I was hoping there would be a way to change it! Guess I redraw then.

What is the purpose of being able to import then if you can't modify?

[JerryFlyGuy]

well if you wanted to import say an iges, and add details you could do that. There is a function to import and then creat features from the import, I've never used it and am not to familiar w/ it. Importing is simply there to help you bring over another program file type and do more work to it in your current software. Kinda like making GMC parts fit a Ford Truck, wouldn't make alot of sense to make them fit perfectly, then you'd be in competition with your competition to make the exact same part, just cheaper..

I think there's an answer in there somplace..

Jerry

[cadman]

You can modify imported models in SW, though not by selecting and changing a dimension like you would a sketch created in SW. Keep in mind that when you import a model created in another system, that model is what you would call a dumb model. There is no information in it to tell how it was made, no history tree or anything like that. There are a couple systems that can do this with models from specific systems like Unigraphics importing Catia models.

The main reason shops import models from other systems is because those cad files come from their customers systems. If you and your customer use the same software, great. If not, you can still work with it in your system.

[scubanick]

if you have feature works when u purchased solidworks(office)
when files are imported Solidworks will do its best to make
sketches and features that would have been used to create the model and you can edit those but if you just have the basic Solidworks package then all you get is that dumb model

[DareBee]

If the model is just a rectangle wqith rectangular hole it should only take seconds to reproduce it from scratch in SW.
If it is a more complicated model you can add features like normal; for instance if it needs to be smaller sketch a rectangle in the right position and the correct inside dimension and use extruded cut - thru all - with the flip side to cut selected - now you can change the outside dims as long as you stay smaller then the original.

Dumb models are great for assemblies using supplier parts; eg -putting a gearbox into a machine. It takes less memory and computing power and is difficult to "accidentally" change.

If you need to do this type of work a lot you will want to learn to be efficient with the "feature recognition" tools. For my needs I have always found it easier to change simple features or start over than to use feature recognition but it is needed for some jobs I am sure.

[cadman]

I'm with DareBee on this. I don't use Feature Recognition very much. For me it's faster and easier to recreate the model on my own than use FR. Feature Recognition works great at for basic features like simple fillets, simple cuts, bosses and a few other things but falls short when it comes to things like fillets along multiple edgs. It likes to create a separate fillets for each edge and that can be a long list in the feature Tree.

[One of Many]

I create a new part and after making a large rectangle with a rectangular cut in it. I can't change any dimension. I get the properties windows to come up but the box where I could change the dimension is greyed out.

Is there something I changed?

Yes, it does get to be a pain when importing as a model. I recently used the "insert DXF" function for a complex rachet/pawl wheel I am designing. Not being all that fluent in SW I had to orient the teeth in Acad, then insert it on the side of the wheel. To convert that to dimensions, I just erased and redrew the sketch, one object at a time. That worked, but with time, I'm sure there are other ways of doing these things quicker.

Sometimes you do whatever gets the job done, regardless of being a technically incorrect process to get there.

DC

[DareBee]

A trick that works for a part like ONE OF MANY's that is mostly 2.5d geometry is:

- Import the dumb solid
- turn it into a single view drawing (above would be a top view I assume)
- Save it as a DXF or DWG
- open the dxf as a 2d sketch in a new part
- now all you need to do is use the contour select tool and extrude all the individual components to the correct thickness.

I would figure on dimensioning (or auto dimensioning) the sketch to make it fully defined as well as easily modified/configured to meet your needs.