So this is for the 1% of users who may have a need or use for using fixed entities in a sketch.

I have submitted it as a bug within Solidworks with my VAR.

Now for the explanation and the issues/ bug that is inherent in the software.

Warning grab a cup of coffee.

For a sample of this behavior draw a circle in a new part define it's radius in the left hand dialog box but don't put a dimension on it directly. Then fix the circle in the sketch now draw a line approximately 1 inch long and dimension this line and make dimension 10", now go look at the circle you "fixed" at a certain radius, it has grown by quite a bit although it is "fixed" geometry it has no value associated with it per the software's programming anyways.

Now after that to my issue with this behavior. Import a customers DXF of a profile of something or a flat pattern for that matter into a solid file. Use bring in constraints and dimensions if you want to. Fix the entities because odds are it is not going to be on the origin or fixed in a logical position. Usually not a big deal. You now have a sketch that is "fixed". Right??? Has dimensions, relations and it appears black or whatever your settings are for fully defined. Ok now lets say you add a line, maybe an offset or some additional geometry you need, you make that line at say 2.00" long in your model and want to dimension it to 4.0" actual length. If you watch carefully you will see that Solidworks just scaled your whole drawing to 2:1.

This is a huge problem for people who frequently convert DXF/ DWG's into parts. At least once a week here. I have been trying for four years to track down how we were getting out of scale profiles for our dies. Turns out this is the root cause and has been there all along. We are on 2018 SP 05 and VAR found it on 2019 SP 02. After we went through the KB and found no direct reference to this behavior I'm assuming it is a small problem that no one has really ever noticed.

From our end it was a huge problem we would design our dies based on customer DXF's add shrinkage and pull factors to get a die that would produce parts within +/-.0005 tolerance. Over the years we would occasionally get a die back that was out of spec and the model would reflect a variant change. Scenario, designer opens a saved DXF part profile that has a 1.245 overall height dimension on the fixed drawing. They double click on it for whatever reason and though it is a DRIVEN dimension,(even says it is driven) you can still change it say to 1.250. That just wrecked our master part.

This really may not affect most people the way it does us, I don't know. I am just putting it out there for anyone who might need to know about this. Hopefully someday a "fixed" sketch will be fixed.

As an example of how and why this is such a big deal here is an entry view of a die we have:

Each one of the blocks ranges in the 5,000 to 7,000 dollar price range which if messed up sucks. What sucks as much is each radius is about an hour grind time and profiles go up from there. Typically a die like this just on grinding can be 4-6 weeks of just grinding.

So if you skipped to the end, "fixed" drawing entities might not be really fixed even if you see all fully defined attributes. BUYER Designer beware.