assembly
SOLIDWORKS Forums
7 months ago

Good afternoon. I´m new forum user.

My name is Matias Mittelbach, and I´m have to change my solid (assembly) scale. I read about it, but I couldn´t use the (operation) scale icon.

I don´t know what happend...

Now the hole of this ring part (dim) is dia:275.5 mm and I need to reduce up to dia: 57mm = 0.2868965 or 28.68965%  (I need to modify the assembly proportionally...). Is there anybody who knows how to?. (Sorry my english it´s too bad!)

Thank you very much!

Mechanical Iris Assy:

Categories: Modeling and Assemblies, Assemblies

Last comment By: Kevin Pymm   Thu, 07 Dec 2017 14:41:46 GMT
Re: assembly

Instead of scaling assembly, try to scale every part - one by one.

By: Vladimir Urazhdin  Tue, 05 Dec 2017 20:59:15 GMT
Re: assembly
###### After all: thank you (большое спасибо)!!

I thought to "disassembly" in parts and redim part by part (I think it´s a long way, but...is the way).

By: Matias Mittelbach  Tue, 05 Dec 2017 21:46:39 GMT
Re: assembly

Hello,

I believe Scale, even at the part level, will not get you the result I think you're looking for.

Scale operates on the X, Y and Z axes.

You can either scale all three axes the same amount or apply difference scale factors to each axis.

In your case, to change the inner diameter, you would only scale on the plane containing the plate and the other two scale factors would be 1.0

But scaling to get your inner diameter will also will change the outer diameter, the diameter of the bolt hole pattern and the size of the holes in the pattern.

What I suggest is to create a configuration of the part that needs the two diameters with each configuration having its own inner diameter value.

Then in your assembly, create two configurations for each inner diameter size and select the corresponding part configuration.

This way when you select your assembly configuration of a certain size, the correct part configuration is selected and the correct inner diameter is displayed.

See Help on configurations.

I hope this helps,

Kevin

By: Kevin Chandler  Tue, 05 Dec 2017 22:33:08 GMT
Re: assembly

Hi Kevin.

I do not know if you work with sketchup, but there is a tool that allows you to resize solid.

I need a tool like that, or the same effect. It is obvious that in the case of this assembly I will have to divide it into pieces and resize and we will be able to see what result I get like that.

And thank abuout my english!!

By: Matias Mittelbach  Wed, 06 Dec 2017 10:53:06 GMT
Re: assembly

Could you maybe save the assembly as a multi-Body part, then scale and then save out all the bodies as parts; replacing/saving over your old files. I know that's a bit of a pig's breakfast but seems the fasest way to scale an assembly to me.

By: Mark Dougall  Wed, 06 Dec 2017 11:24:54 GMT
Re: assembly

Matias,

Is everything in your assembly out of scale by the same amount? Including the gear, thicknesses of parts & the CSK holes in the plate? If so you can use the Scale command on each part at part level. Although personally I would just go over every feature in the tree of each part & correct it to save issues further down the line. If not, you will not be able to scale as Kevin Chandler mentioned, as the gear would end up with a tiny pitch & the CSK holes would be M1.72... instead of M6 for example.

By: Kevin Pymm  Wed, 06 Dec 2017 11:29:19 GMT
Re: assembly

Welcome to the forum Matias,

As Kevin Chandler said, you probably want to address the scale issue at the part level. If it was me, I would consider linking the sketch dimensions for features that will be scaled. That way you could scale them, and leave your hole diameters unchanged...and from there create your configurations.

By: Britt Kessler  Wed, 06 Dec 2017 21:38:14 GMT
Re: assembly

Another consideration Matias.

If, as Kevin Pymm noticed, some parts have a standard features (like threaded holes), the simple one-click-scaling will not work and additional manual editing still required. If this is not just a one time job, may be there is a reason to use Equation Manager: create a Global Variable - Scale and link dimensions to the Scale...

Good luck!

By: Vladimir Urazhdin  Wed, 06 Dec 2017 22:44:15 GMT
Re: assembly

Hi Kevin, thanks for answering me

As a matter of act no,  but i so easy apply scale command and after "repair" thickness holes etc etc etc.

But the problem is I can´t find scale command to operate under "solid assy piece" (you know what I mean?).

If I need to operate this command does not appear for solid use (maybe I don´t know how or where to find it)....

By: Matias Mittelbach  Wed, 06 Dec 2017 14:21:28 GMT
Re: assembly

Scale command is available in Mold Tools menu

By: Vladimir Urazhdin  Thu, 07 Dec 2017 13:28:59 GMT
Re: assembly

Hello,

A helpful tool is to use the search box in the upper right corner of SW:

This search box can be used for different types of searches, so if the ">_" isn't shown, click the down arrow to the right of the magnifying glass and select "Commands" from the list (review the other search choices, too).

Type scale in the search box and click the magnifying glass.

I hope this helps,

Kevin

By: Kevin Chandler  Thu, 07 Dec 2017 13:35:04 GMT
Re: assembly

agree with this. using equations saves a lot of time, especially when you have to remodel complex parts a lot.

By: Furkan Koç  Thu, 07 Dec 2017 13:40:51 GMT
Re: assembly

Matias Mittelbach wrote:

Hi Kevin, thanks for answering me

As a matter of act no, but i so easy apply scale command and after "repair" thickness holes etc etc etc.

But the problem is I can´t find scale command to operate under "solid assy piece" (you know what I mean?).

If I need to operate this command does not appear for solid use (maybe I don´t know how or where to find it)....

Matias,

The Scale feature looks like the icon arrowed in the image below. It may not appear on the tab I have it shown but you can customise those & move it to where is best for your needs. As Kevin Chandler says, if you search in the command box, the scale command will appear in the list & you can drag it from there to which ever tab you like or use the eye to let SolidWorks show you wqhere it is located.

By: Kevin Pymm  Thu, 07 Dec 2017 14:41:46 GMT