Lost my work and cannot find it

[jmaustpc]

I am in the country and NO ONE does FreeCad.

Me too, Australian outback, not many people around here of any sort and not many who would know much about CAD.

I know you will think I am an idiot, but I have lost my work.

It's a steep learning curve, but read the wiki and keep at it, it will get easier over time.

Any suggestions??

Your sketch is not valid, at least not for PartDesign WB or most others because it does not describe one single (or sets of single) contiguous faces.

Like Chris said, simplify the sketch. It's best to have more than one more simple sketch rather than one overly complex sketch in most cases.

For example in this case, spilt the sketches by using logic, perhaps the way you might make the object in the real world.
For example
1) sketch the back plate with no details or at least only a few
2) Sketch the fan cut outs in another sketch
3) sketch the bolt holes and slots in the next sketch

Another tip, consider storing values in one convenient location, like a spreadsheet (or for more simple things perhaps just use it in a property where first used) then reference those values where needed with an Expression. FGor example, lets say the bolt holes are 6mm diameter, you can use that value in both the slots and round holes, if stored in a spreadsheet cell then it is easy to come back later and change the value to say 8mm and have the model automatically update everything.

As Chris said, rather than using distance or similar constraint on everything that is the same, just use "equals" constraint etc.

These screen shots are your sketch and the same one in edit mode

Screenshot_20201121_152627.png (10.83 KiB) Viewed 751 times

Screenshot_20201121_152811.png (142.58 KiB) Viewed 751 times

What are you wanting to do with these sketches? I assume that you are going to model the solid in PartDesign.

I will spend a few minutes making a demonstration based on your file...back in a bit

You have

A quick side note of some nice news, all to little of that this year for most of us, over night Chloe had twins! Clover and Hazel, both girls and very cute, my girls have repeatedly been down the paddock cuddling them and giving Chloe food and water so she doesn't have to go far from them. They are so small when new born and their legs seem too long (out of proportion). For anyone less well informed, Chloe is my family's very, very, fat and much loved pet goat! If you are interested I could post a photo in our "Pets" topic?

Jim

OS: Ubuntu 18.04.5 LTS (KDE/plasma)
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19. PPA
Build type: Release
Branch: unknown
Hash: 48d5ab5ebdbbf7a6399ebf3e0b6af36810ac36b5
Python version: 3.6.9
Qt version: 5.9.5
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/Australia (en_AU)

[chrisb]

I could post a photo in our "Pets" topic?

Of course I want to see your yongest family members.

[jmaustpc]

Here is the file

this demo file I just made is inspired by your complex sketch, but not an identical copy since I don't know exactly which dimensions were correct etc. I have included your original sketch for comparison.

X299-Case-4U-Front-Panel-Switches-New_demo.FCStd

(206.64 KiB) Downloaded 23 times

The spreadsheet contains most of the values that are required to define the object, with the exception of the location of the screw hole slots. The location of the screw hole slots is defined by the red constraints inside their sketch. Note orange constraints have an expression, red constraints are just entered as data. SO to adjust their location, just only adjust the red constraints and they will move. Of course I have made assumptions about their location that may well not be correct, like their symmetry etc.

Screenshot_20201121_173846.png (55.56 KiB) Viewed 715 times

You can just change all the values in the spreadsheet, cells except for one which has a value defined by an expression reading a value from another cell (the value that centres the group of triangles over the fan cut out).

Obviously I simply guessed at how many triangular cut outs you want. Be aware that the sketch for the triangular cut outs will be slow to solve since it is rather complex. I have defined these triangle via the radius of their construction circle before they are filleted.

There are many ways you can do many of these steps, I did it this way partly to demonstrate some ways to do things but also I don't know what are your critical dimensions. You have to start by deciding what aspects of the model are the key aspects from which you then define everything else.

An expression can simply read a value from elsewhere as many do in this file, but they can also do operations on that data as some have in this file. For example an expression can define a value as half of another value etc.

Also note that to make the file more robust I attached all the sketches the the "Body"'s axis plane then applied an offset in Z direction via an expression that reads the value of the thickness of the first Pad from a cell in the spreadsheet, which makes all but the first sketch sit at a height equivalent to to top surface of the first Pad. In this case you could have just left them all on the axis plane without an offset and just toggled the "reverse" property of the pockets, but I thought it was easier to read the way I did it.

Note that I have made several sketches, one for each set of "pockets" rather than having one extremely complex sketch. The only one of my sketches that is complex is the triangular cut outs sketch.

This is what the end result looks like.

Screenshot_20201121_195314.png (8.53 KiB) Viewed 715 times

I hope this helps...


Jim

Edit:- you seemed to want to difine the location of the crew hole slots from their centre rather than from the centre of one of their end curves, that is why I added the extra construction geometry (dark blue line) to the slots.

[foxint]

Hi

Thank you, all the replies. They all sounds great, but you lost me.

The sketch is the front of my PC the holes at the edges are to screw it into a 19” rack the larger circles (will be removed as they show the position of the fans) and the 4 holes are 2 switches and 2 lights. The triangles are the vents through which the fans pull air into the PC Case.

ChrisB suggested (mirroring that I made a big mess last time), so I spent all today and most of the early evening doing 50% of the holes.

I have tried as much as I can to incorporate what I understand. As for the term’s symmetry (I think I understand make the triangles relate to each other – somehow).

The spreadsheet sounds great, but I do not understand a word you have written.

I found that my little triangles were all different sizes. I set up one and then I copied and pasted and for some reason they all were the wrong size. I had to start again.

So, I set up a group of 10 triangles. I copied and pasted each group of 10 and still they changed size.

As the project got larger, I deleted the set of triangles, to keep the power draw to just Very High…

Each time I move and located the triangles many changed size and some dramatically??? I even had a triangle turn into a Celtic knot…Also the triangle should be symmetrical, but there must be a rogue measurement…. (they stick out too much at the top).

Not sure what to do. I did manage to do 50% of the ventilation holes. The PC crashed 4 times and I decided to only run FreeCAD. It remains terribly slow…. It has taken me from about 9am to now about 8:30pm…. May be a faster PC with more RAM. Ha-ha… (now almost 9pm)

I now save after each action is completed. Even deleting takes a long time.

Perhaps someone has an easy way for me to fix the 50% I have done and replicate this to the other side. Something really dumb so I can understand it.

I was hoping to send the file (and others that are baby-stuff for you guys) to the laser cutter soon.

Thank you

Dummy from the Bush

[chrisb]

Look at how Jim modeled the triangles. Here is another way where the arcs of the triangle corners are tangent to the outer circle.

Snip macro screenshot-bbafd3.png (16.59 KiB) Viewed 702 times

Please note that a sketch can only be padded if it contains no more than one level of nested closed paths. The edges must not cross nor form a T-joint.

[foxint]

Hi ChrisB

Thanks for the reply

I used the triangle tool. But then when I changed to parameters, the circle around the triangle was not attached. So I removed them.???

“Please note that a sketch can only be padded if it contains no more than one level of nested closed paths. The edges must not cross nor form a T-joint.”

I do not understand what you have said.

[chrisb]

I do not understand what you have said.

What is it what you don't understand? Levels of nesting? Crossing lines? T-joint?

[chrisb]

• These can be padded:
  No nesting:

  

  Snip macro screenshot-0b9681.png (1.36 KiB) Viewed 649 times

  .
  One level of nesting:

  

  Snip macro screenshot-6d6ab1.png (7.26 KiB) Viewed 649 times

• These cannot be padded:
  2 levels of nesting:

  

  Snip macro screenshot-7b4d8b.png (1.71 KiB) Viewed 649 times

  .
  Lines crossing:

  

  Snip macro screenshot-a81a09.png (1.55 KiB) Viewed 649 times

  .
  T-joints:

  

  Snip macro screenshot-2f2ad9.png (1.44 KiB) Viewed 649 times

  .
  Path not closed:

  

  Snip macro screenshot-c556e8.png (2.16 KiB) Viewed 649 times

[jmaustpc]

Read the forum rules link at the top of this forum, one of the posts in it shows you how to use the forums quote mechanism.

, but you lost me.

Well any CAD is a steep learning curve if you know nothing and start with something a little complicated and you will not read the wiki!

The sketch is the front of my PC the holes at the edges are to screw it into a 19” rack the larger circles (will be removed as they show the position of the fans) and the 4 holes are 2 switches and 2 lights. The triangles are the vents through which the fans pull air into the PC Case.

Well why didn't you say that the first time? I can't read your mind, only look at what you did and guess.

so I spent all today and most of the early evening doing 50% of the holes.

Well that is ridiculous, you would have been better spending half that time reading the instructions in the wiki.

So, I set up a group of 10 triangles. I copied and pasted each group of 10 and still they changed size.

“Please note that a sketch can only be padded if it contains no more than one level of nested closed paths. The edges must not cross nor form a T-joint.”

I do not understand what you have said.

You make it hard to succeed when you refuse to learn first the most basic principles of how sketcher works, its not 2d CAD its a constraints based sketcher.

Of course your triangles resized, if you have not first constrained everything except its location then anything can move in any way. When you drag the triangle an edge can be extended or the whole line can move but if you had first constrained the length of that edge and then dragged it, then it would just move and not resize.

Understand these principles before you try to do anything.

1) geometry is described in sketcher by a set of constraints and some basic features, e.g. basic feature: an edge could be an arc or a straight line e.g. of constraint: - the length of and edge from one point to another. When you first enter geometry you get some default features and some automatically added constraints, but not enough to fully describe the geometry you entered or its location.
2) there are two fundamental types of geometry, standard and construction geometry. Standard geometry shows up as a a real edge when the sketch is not in edit mode and can be used to create solids in PartDesign workbench. Construction geometry is invisible when the sketch is not in edit mode and is only used as a helper or guide for other geometry and is blue when the sketch is in edit mode. So you should have drawing your fan circles in Construction geometry.
3) what Chris was talking about with the faces and nesting. The finished sketch must describe the outer edges of a face, which can have holes, but not a hole inside another hole, and if the edges overlap FreeCAD can not determin which is supposed to be face material and which is supposed to be a hole. E.g. A sketch with a plain square would describe a square face, so PartDesign Pad would produce a cubic solid. No consider if you put a circle in the middle of the square, you Pad (all Pads must create a single solid) that and you will get a cube with a round hole in it. Now what on earth do you think FreeCAD would do if you had two circle one inside the other? which is hole and which is material? FreeCAD can't tell, if the edges overlap you have the same problem. This is really basic obvious stuff, just try a simple sketch yourself and you will understand.


As far as your triangles go, they have a blue construction circle, all their points use point on edge constraint by default on first creation, so if you make the circles the same size (just select the blue circle and apply the "equals constraint") then they will all stay the same size.

You then tried to make curves at the triangles' points (called a fillet) but by doping so you deleted the point on edge constraint because that had been one the two points on the ends of the adjacent edges. So what I did was convert the triangles into construction geometry then constrain the new normal geometry edges and curves to that construction triangle. Chris is suggesting another method to end up wit hthe same end result. There are often many different ways to get the same result.

Regarding the spreadsheet, it just hold values for convenience, those values are used in several places where instead of entering a value directly e.g. 15mm, I have added an Expression which reads that 15mm from the spreadsheet cell. Don't bother trying to understand expressions just yet you are obviously way too much a beginner.


Don't waste so much time again doing something you are just not understanding, next time read the wiki, go back to doing something more basic until you understand how to do the most basic things first, and ask here on the forum.

[jmaustpc]

Chris and I were typing at the same time. hence our last posts have duplications.


Another though, why are you using triangles at all? Is there actually a good reason? if not and they are only for air flow, then consider a much simpler shape like a series of circles, or perhaps slightly more complex use squares.