Why is the tool slow on my system?

H4NNE5

Hi, I just started using Onshape 2 weeks ago and i now have a very simple design: a hole matrix of 31x11 holes.
Opening and working with the document takes very long. If I want to draw a new shape I have to wait like 5 seconds until it appears after I made the line or circle with my mouse.
There is the small "loading" symbol at the bottom rotating for a while. I'm just working in the sketch.
Could there be a limitation in the speed of my internet connection?

Best regards
Hannes

3dcad

Can you make your document public and share a link here for others to test?

rbaek

johannes_hofmann763 said:

Hi, I just started using Onshape 2 weeks ago and i now have a very simple design: a hole matrix of 31x11 holes.
Opening and working with the document takes very long. If I want to draw a new shape I have to wait like 5 seconds until it appears after I made the line or circle with my mouse.
There is the small "loading" symbol at the bottom rotating for a while. I'm just working in the sketch.
Could there be a limitation in the speed of my internet connection?

Best regards
Hannes

How did you create the hole matrix? Did you use the hole feature or did you use a combination of other features?
If it's blocking you from working on your document, you can use the restore functionality in the history flyout and revert back to the state prior to when you made the change that caused this to troubleshoot this.

H4NNE5

Hi guys,
I hope this works as the link: https://cad.onshape.com/documents/5bd015053ae8426499cb81c4/w/b0b272da5d0b4f6099f8a50e

I made one cutout and used the pattern tool.
It didn't get slow in an instant. I had the feeling that with the size increasing the speed dropped.
The file size is 129MB now. I have no reference of how large a 3D file can get.

rbaek

H4NNE5 said:

Hi guys,
I hope this works as the link: https://cad.onshape.com/documents/5bd015053ae8426499cb81c4/w/b0b272da5d0b4f6099f8a50e

I made one cutout and used the pattern tool.
It didn't get slow in an instant. I had the feeling that with the size increasing the speed dropped.
The file size is 129MB now. I have no reference of how large a 3D file can get.

Was the cutout created using hole or another feature?

H4NNE5

I used the circle tool and then modified it with lines.
But today i also logged in from my company and it was similarly slow as on my home system. And my company's internet would not be a limitation
So i have to assume, that the lag is caused by the Onshape servers.
I use Chrome btw.

3dcad

@H4NNE5
It did load a bit long but once it was ready I had no problems manipulating the view. But when I tried to edit dia of the hole, it took so long that I closed the window. Experiment with cheap chromebook.
You can reduce size of any document by making a copy (this will purge edit history) and my copy was 'only' 20mb.

Onshape doesn't need that much bandwidth after model is fully loaded, you can work even with 3G. Complex (or otherwise demanding) designs enjoy big RAM and flawless viewing requires decent graphics card.

I will give this a try with w10 pc tomorrow at work.

ps Tervetuloa..

PeteYodis

The more efficient way to handle this, as well as with your current MCAD products that I am familiar with - is to make one hole cut with one sketch instance, and then use face pattern to conduct the 11 X 31 pattern.  Putting that many pattern instances in a sketch is begging for trouble.  I think you will see performance is much improved if you keep the sketch as simple as possible.  That was always my rule of thumb as a designer.  Keep sketches as simple as possible and at bite size pieces.  I'd rather add a new feature to the tree than add too much complexity to a sketch.  Try it and let me know here.

øyvind_kaurstad

@PeteYodis Does that also mean, in your opinion, that it is often better to create new sketches for new features, even if the new feature could be made by first adding something an existing sketch? I regularly find myself in that situation, and I am often unsure which method is the best. One point to make is that adding to an existing sketch might cause something to break, like an extrusion of certain sketch features (if the newly added sketch entities interfere with the existing). To fix, one then has to edit the extrusion and correct which faces are used. Easy enough, though.

PeteYodis

It depends on the situation, and sometimes it is also a matter of organizational preference.  When I knew I was going to be pushing the sketcher, I would back off a bit.  It is somewhat akin to personal preference on how you want to organize your sock drawer colliding with things you just shouldn't do.  You'll get a feel as you do more.  I think the performance issue you are bumping into on the sketcher is the constraint manager handling all the relationships of all those entities.  There is a lot for constraint managers to do in sketchers when you heap that kind of load on it's back.

PeteYodis

Also, for people concerned about the robustness of the face pattern, this can be overcome by patterning a cutting body and then performing a boolean.  This would be robust if the pattern faces were severely affected if things were changed upstream in the tree.

H4NNE5

PeteYodis said:

...make one hole cut with one sketch instance, and then use face pattern to conduct the 11 X 31 pattern...

I don't understand that part. I made one cutout in the sketch and the rectangle. Then I used the pattern generator to multiply the cutout.
What do you mean exactly with your manual (to me it sounds exactly the same what I did)? Please explain step by step  

@3dcad: I copied the workskpace and now it's only 7MB! That history was creating a huge overhead. Can I "delete" the history if i make it a version or sth?

3dcad

@H4NNE5
You did pattern in sketch ie. you patterned sketch figures and then chose to extrude them all. Pete is suggesting to draw only one shape in sketch, extrude that and the select face pattern in modeling tools and select all faces of that extrude and set pattern values.

Only way to purge history is making a copy and put the original in trash and empty trash. Please remember that 'file' size updates with delay.
You can find a lot of conversation on this at different discussions in this forum if you wan't to 'join the choir'.

PeteYodis

Have a look here.... https://cad.onshape.com/documents/5595a1cdb1d24fe6ab0d2397/w/db21a46f875f4f95bb335ac3/e/8064eee1169146f197b3ff66

I'll add another branch where I use a boolean pattern remove combo...

PeteYodis

okay... look at this branch in the document to see the other method...