scaling inside the sketch environment

[Sungod3000]

Hi,

Im working a lot with offset in sketches to keep tolerances on my 3d printed parts.

So I sketch out something, add an offset of x, continue and then start finetuning an that includes scaling.

AFAIK I can only scale the whole sketch, that unfortunately means that my offsets also get scaled.

Is there a way to scale inside the sketch environment? I tried just selecting and dragging certain parts like eg a circle but that deforms the parts because I cant lock the dimensions.

[Phil.E · Accepted solution]

There currently is no scale command in the sketch environment.

1. I would suggest creating a unitless user parameter: Scale = 1
2. Then for the shapes you want to scale, add this to the dimensions, like this: X.XX mm * Scale
3. When you want to change the scale of the dimensions, edit the parameter for Scale.

I just did this in a couple minutes. It works well. NOTE: fully constraining the sketch is required.

Thanks,

[dghylin]

Phil,

Just learning this so this may be a pretty simple question but...I've created a parameter and using a simple rectangle in a sketch the parameter works but just for the dimension I edit.  Not sure how to "fully constrain" this sketch so that both verticle and horizontal scale at the same time.  Any help would be appreciated...

Don

[MattPerez314]

Don, he means the sketch needs to be related to the origin. The example of the rectangle, a center point rectangle coincident with the origin amd that has horiz/vert conatrains on all sides or one side and perpendicular between all the others. This way the dimension change is conaistent.

For the challenge you will need to go to modify/change parameters. Your user parameter foe scale, lets call its ScaleFactor, has a value of 1.11. In your sketch when you dimension your length and height(lets say 10 & 5) you will enter "ScaleFactor * 10" for length and "ScaleFactor * 5" for height. You need to know the parameter name and its case senaitive I believe.

Ps sorry for any typos, im on my phone

[Phil.E]

@MattPerez314 Great answer, and yes parameters are case sensitive.

@dghylin Take a look closely at the screen shot I provided. In the parameters dialog I multiply each dimension by  the paramter Scale. So a vertical and horizontal dimension on a rectangle would both be multiplied by the same factor, and thus both change together if you change the value for Scale.

When I say "fully constrained" I mean that each line, arc, or circle is defined by dimensions or geometry constraints. If one line (in your question it would be one of the sides of the rectangle) is not dimensioned, and thus would not be multiplied by Scale, it would make a huge difference.

I hope this helps, let us know if you have more questions about it.

Thanks,

[dghylin]

I'll look at the example and these posts more closely.   In the mean time, I found a work around that does what I'm trying to do. The problem I see is that the sketch is an inserted dfx file that is comprosed of lines that are not always perpendicular and horizontally.  The sketch may include curves, circles, elipssis, etc.

First, I insert a dfx file into the sketch window (this, for some reason does not come in dimensionally correct).  I think either me or the program is confusing mm and inches.  Then closing the sketch window and push/pull to obtain an object.  I scale that object, delete the sketch and create a new sketch window on the side of the object.  Then I delete the object and using the new sketch (now scaled to the correct dimension overall), push/pull to obtain a correctly scaled object that is tied to the new sketch....hope that all makes sense, I know it works and probably not the fastest or the easiest way to get there, but, I'm retired and have the time...:)

I've attached a file showing how I do this, although I did not delete the original sketch window in this sample.

http://a360.co/1Q5wcMd

Just a test for an old guy to learn as much as he can in the time left, so don't be too critical on the design...lol

Thanks all for the input,

Don

[Phil.E]

@dghylin

For the units problem on insert: check the units of your environment when you insert. If the file was created elsewhere, it should export with the native units. Fusion 360 will use those units in the environment you insert into.

So if you have an "mm" dxf, and insert it into an "inch" Fusion design, it will likely be 25.4X larger than it should be.

Thanks,

[dghylin]

Phil,

The original was developed in DraftSight, in inches. Saved to dfx. Then inserted into the sketch pane (with Fusion setup in inches). I think there is some formatting in DraftSight that I'm missing. Also, there are many dfx settings to save to, is there a preference as to which one to use?

Don

[Phil.E]

Does DraftSight have the concept of "export units"?  That's a possibility. Also, not everyone uses the DXF standard to carry units. Not sure if DS is such a thing.

You might try changing Fusion to CM and then importing the DXF, then changing back to Inch. See if it's the same size. It's a units mismatch and CM is the native unit for Fusion, so that's a good place to start.

Thanks,

[dghylin]

Still doesn't scale correctly. The original dwg scales to 32.2564". When inserted into sketch pane of Fusion (set to CM) it reads 32.046 CM...then changing CM to Inches in Fusion everything re-scales everything and reads 1'-45/64"....strange...I'll investigate DS a bit more. I though we had this problem solved last week but then DS upgraded and I'm not sure what's going on.....thanks for the help anyway, will post if I find the problem...

Don

[Phil.E]

That is odd, and not a units mismatch. It's too close.

It almost gave you the exact as-designed result: i.e. it should have been 32.2564 CM, just transposing inch for CM.

Try with some test shapes, exactly 10 inches in one direction is perfect. That way you can see really clearly if it's a units problem or some other scaling issue. Feel free to attach the file here, I'll have a go.

Thanks,

[dghylin]

OK....here's a Fusion file of a Clark Y airfoil that was drawn in DraftSight with a 10" cord.  Have also attached the .dwg file and the .dxf file of same.

It exhibits the same dimensional characteristics as the previous post but it's only .001 off. 

Hope you can determine what's wrong here..

http://a360.co/1QIZh3r

Don

[dghylin]

Phil,

Still can't get Fusion insert to work correctly...i.e. to the correct dimension, but have another work-around which is fairly easy.  In my CAD program I just scale part up by 2.54" and that dxf inserts in Fusion sketch with correct measurements. 

Don

[MattPerez314]

Don, in draftsight what is the setting under "format>Unit System" ?

[dghylin]

Initially was set to "Unitless" but I reset it to "Inch"....still won't insert correctly into Fusion Sketch....

[Phil.E]

My guess is when you created this file DS was set to Unitless, which in the DXF file generic units are actually CM. At least that's what Fusion 360 is reading from your files.

It imports to Fusion 360 perfectly as 10 CM. There are no rounding errors.

When inserted to Fusion 360, while Fusion 360 is set to Inch, it is perfectly 10 CM converted to Inch. (~3.94")

Which means that the DS file is in CM and Fusion 360 is reading it properly as such. Units are being read by Fusion 360, they are CM in the file.

This also opens in ACAD as exactly 10.000000 units. And if I set Insert Units in AutoCAD to "Inch", then export it from ACAD to Fusion, Fusion reads it as 10".

So your workaround of scaling everything in DS by 2.54 is the only correct workaround for you.

Another thing you might try is creating new files in DS with the Inch units setting that is mentioned above and see how Fusion 360 imports it. Let us know how it goes.

[dghylin]

Phil,

I created a completely new drawing, made sure all the settings were set to inches and saved to dfx...tried inserting it and got the same results as before.  It appears DraftSight doesn't understand Fusion or visa versa.  I'll just stick with my workaround of scaling up in DS prior to saving off the dfx.  Really not a big problem.

I do have one more question that might be related to this issue though.  I've attached a .png of the various settings available when saving in DS.  The highlighted one is the one that I use mostly.  Could this possibly be the problem and if so, which setting should I be using?

Thanks to everyone for the help,

Don

[Phil.E]

I don't think it makes a difference. Here is a good explanation of binary vs ASCII dxf files.

http://www.autodesk.com/techpubs/autocad/acad2000/dxf/binary_dxf_files_dxf_aa.htm

Good luck and please let us know if you have more questions.

[dghylin]

Thanks for the response Phil, I pretty much have settled on just scaling up in DraftSight.  But, next time I have an hour or so to waste, I may try each of those dfx types just to see if one might work correctly.  Right now I'm struggling learning other aspects of  Fusion.  So far, so good....:)

[dghylin]

Phil,  I think I've found the answer to this scaling problem.  As mentioned above, had an extra hour so I sat down and tried a few of the different dxf file formats and found two that do work correctly.  Either the R2013ASCII or the R2013BINARY formats translate dimensionally correct across from DraftSight to Fusion360.  I found those two that worked and ended my search....two will be more than enough, just have to remember to select one of those when saving to dfx.  Problem solved!

Thanks for your help and all the others posting in the thread...much appreciated...:)

Don