Relations

Can anyone share a the quickest method of deleting all relations in an entire model?

In my position, I seem to have to continually remove features to get some features I want, but the relations sometimes are a real pain because it won't let you remove features.

Reply to
Bill Cain
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Bill,

I would suggest that you're going a bit overboard. At the risk of sounding rigidly absolute, deleting all sketch relations in a model strikes me as a really bad idea. There is no tool in SolidWorks that allows you to do that, unless you wrote a macro to do it. You can delete all the relations and dimensions in a single feature using the Display Delete Relations tool.

A better approach, from my way of thinking, is to get more comfortable with building with a "design for change" concept. If you delete all relations, the very next change you make, you're going to wish you had them back.

There are many examples that can be made, but one of the most frequent is when folks put fillets on early in the model, then sketch relations in subsequent features go to the edges of the fillets. Now you're trapped. Cosmetic fillets are better off going at the end of the tree. Non-cosmetic fillets have to go where they have to go, but consider making sketch relations to the sketch that made the edge (for extruded features) rather than the edge itself.

Modeling this way takes a bit of discipline. It's not as fast as clicking on a face, hitting convert entities and extruding. The concept can be carried out to its theoretical extreme where a skeleton of the part is made from sketches, planes and axes, and the solid features have no relation to one another, only relations to the origin, sketches, planes and axes. This is an extremely conservative approach, but also valid way of doing things. If reliability through changes is your main concern, the more conservative you are, the better. If sheer initial modeling speed is the main concern, then "fast and loose" use of all the design automation tools is what gets you there.

Nobody's going to tell you how to model, but different techniques are good for different goals.

Reply to
matt

Matt said a lot of things I have learned the hard way (and fortunately don't need to relearn too often). The acid test of a CAD designer isn't what he can model, it's what he can change.

I spend a fair amount of time laying down foundation or framework before any solid features are made. When I designed hinges, all parts had skestches, planes, and axes indicating pivots, mounting surfaces, and overall profile before the first soli feature was made.

Once your layout/skeleton features are in place, refer to them whenever possible. i.e. Don't use a face edge when it coincides with a layout line; use the layout line. this way you don't have references stacked

10 deep that unravel when one feature changes.
Reply to
That70sTick

Hi Matt,

Thanks for the advice. I am an applications engineer for a CAD/CAM company. Hence I am not really doing much as far as creating models. What usually happens to me is, I get a model from a customer who wants advice on how to use our software to machine a specific part. Ocasionally, to get the tool path I want use, I have to modify the model or more often delete some features. What i keep running into is the feature I need to delete is releated to something else and it won't let me delete it. At this time, I also have no formal training in solidworks. I will look at the Display Delete Relations Tool as it sounds like that may help me.

Reply to
Bill Cain

Bill,

Deleting relations, especially in a sketch can cause performance problems as well as leaving the model totaly free to move around.

Bill Ca> Can anyone share a the quickest method of deleting all relations in an > entire model?

Reply to
TOP

Bill,

Cleaning up a part so that it can be machined or have other processes applied is a bit of an art. The tools of the trade are suppression, roll back and reordering. There is a parent/child tool that can be invoked by right mouse clicking on a feature. This will show how a part is modeled in terms of dependencies. You can do various tricks also if you have the Utilities addin like search for features of a certain size. You can use a surface to remove features also. Since we don't know what process you are preparing the model for I can't be more specific.

You might also consider exporting the part into a parasolid and reimporting it. Then use various cuts to remove material you don't need on the dumb solid. In this way you won't be in danger of accidentally modifying the customer's part.

Bill Ca> Hi Matt,

Reply to
TOP

Do some experiments with dumb solids. Export your part as a parasolid, re-import, and see what you can do with it.

Things to try:

--Delete Face

--Replace Face

--Move Face

--"Drill-and-Plug": cut out a region that doesn't work for you and replace with your own geometry. Sometimes helps to save original faces first using offset surfaces to use as reference for your new geometry. Use "Delete Bodies" to clean up extra surface bodies afterward.

Reply to
That70sTick

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