PC stalls and takes up to 25 mins to make changes

[foxint]

OS: Windows 10
Word size of OS: 64-bit
Word size of FreeCAD: 64-bit
Version: 0.19.17505 (Git)
Build type: Release
Branch: master
Hash: 755536e9df94d2d39da1468420f1fd333c35da7a
Python version: 3.6.6
Qt version: 5.6.2
Coin version: 4.0.0a
OCC version: 7.3.0
Locale: English/Australia (en_AU)


Hi Guys

Thanks for all those who have had the patience to solve my problems.

I have another, but it is more of a PC resource management issue.

As the file in FreeCad gets larger, the time it takes to do anything increases. Currently I have been waiting 5-20 minutes, just to make an adjustment in a straight line length. 5 mins is not uncommon if I am checking a measurement.

Currently I have waited 25mins and it is time to pick up the kids from school….

Any clues. I have shut down everything. My task manager says:

CPU Usage 10-16%
Memory 227.7 MB

Says the programme is not responding.

It is very annoying.

I have 64GB of ram a 2011 socket i7 on a Gigabyte UD5 board. Not new, but still good.
Graphics Card: NVIDIA GeForce GTX 560 Ti

Is it the graphics card????

I have attached the file.

Thank you all for reading this

D

[Roy_043]

I am by no means a specialist, but the large number of constraints (1399) is probably the main problem.

[papyblaise]

Hello
I redo your drawing in 2 separate sketch , plus 2 patrn array , and the modifs Don't lost time

[foxint]

Hi Guys,

My apologies, I was stuck down with a 24hour gastric episode. Now only have the headache.

Thanks for the comments.

Roy_043 – as I am a novice, I thought that to limited the degrees of freedom of the design would allow me to move parts without distorting the compound shapes. I thought that limiting degrees of freedom makes for a more precise and robust design. Obviously there is a problem

Papyblaise – Salut…merci, but you have totally confused me. I cannot work out how to change or modify the drawing. Looks great thank you.

Yes…still confused. I am learning, but surely my little drawing should not have caused the process to stall???

D

[vocx]

... I thought that limiting degrees of freedom makes for a more precise and robust design. Obviously there is a problem

The problem is that your figure doesn't require that many constraints. Your body has a pattern that repeats many times the same shape, that is, the hexagon. Instead of creating many hexagons, and constraining each of them, you can create only one, and then use arrays to replicate the same feature many times. This is easier than what you are doing currently.

A sketch uses what is called a "constraint solver", which basically defines many mathematical equations, and then solves them. When you were in school it took a while to solve by hand a linear system of equations with 4 equations and 4 variables, right? So, think about solving a system with hundreds of equations. Every constraint that you add adds more equations to the model, so minimizing the number of constraints will reduce the amount of work the solver needs to do. Every time you try to modify even a single line, all equations need to be solved again, so it's going to be slow once you add too many constraints.

When working in CAD, you want to minimize the amount of effort it takes to produce a shape. If something can be defined in simple steps, that is preferable than using complicated techniques; this generally means using simple sketches with few constraints, whenever possible. Only experience can tell you if your modelling is good, or bad.

Papyblaise – Salut…merci, but you have totally confused me. I cannot work out how to change or modify the drawing. Looks great thank you.

What he did was to use the Part Workbench, not PartDesign Workbench. He used a basic sketch to draw the base, then he used another sketch to draw the hexagon, then he used Part Extrude to produce solids, and then he created a pattern using Draft Array. Finally, he cut the first solid using the second solid (the pattern of hexagons). This way of working is called constructive solid geometry (CSG), and it's the traditional way of working in older CAD systems. Expand the "Cuts", "Arrays", and "Extrudes" that you see in the tree view to get to the original Sketches that produce the basic shapes.

In PartDesign you can do the same, but with native tools of PartDesign, such as PartDesign LinearPattern. Instead of boolean operations like Part Cut, you use a PartDesign Pocket. I suggest you take a look at the Tutorials page to learn more about the PartDesign workflow before proceeding further.

[foxint]

vocx

wow....thank you. I am totally confused. Will try and read some more. The onion, just keeps opening and I keep saying WTF....

will try and make sense of what you have said.

Great comments - thank you

D

[chrisb]

To make things clear: The previous posts suggested to limit the number of constraints. I would like to point out that it is still very much advised to fully constrain sketches. So the suggestion goes hand in hand with the other advice given to simplify the sketches.

Concerning the pattern function in PartDesign, which are the counterpart of the Draft->Arrayfunction used by papyblaise: They work and are comfortably to handle, but they are currently utterly inefficient. The models become rather big, and - worse for me - become very slow in recomputing. The honeycomb here may already be beyond the limit, so it was sensible in this case to use the Draft array.

[foxint]

Hi chrisb

Nice to see you again.

Thanks for the comments.

I did try to open the new file in Part and in Draft and nothing. I am going to have to go back to the side-lines and later try and workout what “papyblaise” has done.

I went down the complete list of (I think they are called) “work benches” as was unable to modify the drawing.

If as you said my honeycomb is beyond the limit, would a new graphics (second-hand good one) would make life a little faster???

I am going to sand some metal and get my frustrations under control.

Thank you
D

[chrisb]

Papyblaise's model is made in Part workbench. You can modify it by selecting an item in the tree and then change it's properties in the Data tab at the left lower side.

[foxint]

Hi Mate,

Thanks

I think I have it in edit mode - totally different from sketch (or have a made a mistake - probably made a mistake).

Lost me.....

D