svg

[Anonymous]

Hi, I've lost a thread answered by Jeff.

Project: To construct a shell with a hole in the top face in the shape of an imported svg sketch and produce a 2D Eng Drawing.

Problems: Imported svg is very difficult to select to unfix. A selection box leaves parts unselected. It took quite a time to expand and select missed nodes/sections.

Scale: incorrect on import but notepad shows file in mm. To get it to an exact size was a laborious job consisting of end to end measure and calculate scale factor. Dimension tool wouldn't work as I couldn't select the sketch after choosing Dimension.

Positioning: It seems moving is relative to current position rather than by coordinates.  Following the insertion of a previously drawn shell I was able to move the sketch to a random position on the face but it then became unselectable when trying to cut the hole. Undo to the sketch, pull the sketch and move back onto shell as a body (into a random position) then use combine to 'cut' the hole. I tried to use align but had selection problems.

I would like this project to be simpler. I expect to be able to import an svg sketch, unfix it in a single operation then scale it to an exact size by entering dim mm, move it to an exact position on the required face and cut the hole.

So far I'm into the 4th week and have got so confused the learning of the software outside of this task has fallen by the wayside.

Can someone point me in the right direction?

[innovatenate]

Is this the thread you're looking for?

http://forums.autodesk.com/t5/sketching-sculpting-modeling-and/modify/td-p/5716882

What is the SVG file for? A logo? Could you post a screenshot of what you are working with? I'm wondering if the SVG file could be split up into smaller files or if you could use symmetry or something to reduce the size of the SVG. From your comments, it sounds like the SVG file is really slowing things down.

Thanks,

[Anonymous]

Thanks for the thread link.

This svg is an 'ACE of Spades' shaped drawn in Corel draw x5 and exported as an svg.

It is to be used to create a hole in the face of a container for a pack of playing cards with the hole precisely corresponding

with the printed shape on the pack.

Following the import the svg cannot be selected until each individual segment has been unfixed. Pulling a selection box around the shaped fails to select all segments.

(is it not possible to group all segments to form a single entity?)

Once completely unfixed it is then possible to select, move and scale the shape. I have now managed to place it onto a previously constructed shell but then found it impossible to reselect it to extrude/cut the hole. However, by extruding prior to positioning I have been able to use combine successfully.

The questions remaining are 1, is it possible to size the shape formed from the svg by entering values directly?

and 2, how does one precisely position this shape onto the face of the shell?

[innovatenate · Accepted solution]

The sketch environment inside of Fusion 360 can use sketch dimensions, constraints, and even parameters to control a sketch. However, it is much easier to build these relationships natively in the Fusion 360 sketch environment, than it is to import the sketch and try to create relationships between sketch entities (e.g. dimensions & constraints) afterwards. During the import sketch entities may be converted to a spline, which are difficult to dimension.

I think the strategy of using the scale and move commands is the correct one in conjuction with an SVG file. A couple of thoughts on this are:

The Insert SVG command has the ability to Move and to Scale built into the command. Prior to inserting the SVG file, create another sketch that may serve as a bounding box for reference. Now when inserting the SVG file, you can populate the scale &  X/Y position fields to size and locate the sketch entities.

In order to Move or Scale the SVG after the insertion, all of the sketch figures will need to be unfixed. You should be able drag a selection box around the sketch entities to select them all.  One thing to be aware of is if you move the select box from left to right versus right to left, you will get a different selection box:

• The left to right selection box (solid line/orange)will only select entities that are entirely encompassed in selection box. 
• The right to left selection box (dashed line/yellow)will select entities that are only partially encompassed in the selection box.

Could this explain why you're not able to select all of the sketch entities at one time?

I would also note that the Move command has a Point to Point option that can help you precisely position sketch figures. 

See a Screencast of Move Point to Point in Action.

http://autode.sk/1OCEsl9

One thing you will note in the above Screencast is that after moving the sketch entities, there is an orange "infill" between the sketch entities. This indicates that the sketch entities are enclosing an area. This will be key if you'd like to use the profile in an extrude cut feature. 

If you do not see the colored infill to indicate a profile or an enclosed sketch area, this indicates that there could be a gap or an overlapping figure. 

One trick to finding these gaps or to working around these gaps is to use the Patch > Extrude command. You may then begin to work with surfaces in 3D, despite not having a Profile.

I hope this helps. Please let me know if you have questions or concerns. If you can share the SVG file in question, I would be happy to take a look at it. 

Thanks,

[Anonymous]

Many thanks, your response has provided more insite into the handling of svg imports.

I have managed to stumble my way through to a printable model but I will start again taking onboard the points you have clarified.

[Anonymous]

Nate, I try to import SVGs and at the end of the command a warning box comes up saying the file is invisible, toggle visibility in the browser, but its nowhere to be found in the browser.. what could I do?

[innovatenate]

Are the light bubles for the sketch folder and the sketches in the sketch folder yellow? If not try clicking on the light bulbs to toggle the visibility.

Hope that helps!

Thanks,

[Anonymous]

Thanks for the quick response!

Yes I is yellow, the command creates a new scketch but this new scketch consists only in the contour of the component I selected when choosing plane for the SVG , even if the SVG itself was bleeding over the plane of the component.

[innovatenate]

Could you post a screenshot? It may give some further clues.

[Anonymous]

I captured a video of the issue, is there an email or any other way I can send it to you?
the Quicktime video file won't gett loaded through here...

[innovatenate]

Can you e-mail it to support.fusion360@autodesk.com? In the future you may want to check out Autodesk Screencast as a recording utility. It works really well and provides some additional Autodesk specific support, like a timeline of the command that you use. 

https://knowledge.autodesk.com/community/screencast

Thanks,

[Anonymous]

 I cannot get an SVG file which is text on a path from AI to do anything but import itself way off 0,0 and it cannot be moved.

[Anonymous]

I am having a similar issue with SVG files. 

Once imported, the file clings to a set profile plane, that will not allow me to use the offset of the trace to extrude. 

I am offsetting the exterior edges to extrude, because I can not expand the profile plane it does not act like it is all the same sketch. 

My goal is to create two offsets to perform extrusions to the outer offsets. I usually just trace the image, but find it much easier to get a better-completed product if I can use the SVG files to complete the task. 

My question would be either to expand the offsets to be included in the profile plane, or a way to add the offset traces after the fact into the sketch.

sketch 1 shows you the problem area in blue. 

sketch 2 shows you a closer view. I am unable to extrude the areas that are not pink (or blue when highlighted). I am trying to get a plane between the lines. 

[davebYYPCU]

Extrude needs a Profile - the shaded orange in that single pic.  

There are two offset curves above that are not shaded, will not extrude as a solid, but you may get a surface extrude as it is. 

Usually means there is a hole in the outline, or the curves are in 3d.

Might help...

[Anonymous]

Your quite right. Sometimes for example if you add two lines to create a rectangle in the corner of another rectangle which was created with the rectangle tool. The inside rectangle appears to be a selectable face but it’s not.

I do sometimes wish that preferences gave me the option of leaving a sketch OPEN after extruding a face within a larger sketch. Especially after I’ve done an SVG trace for instance. It would be a step saver.

Thanks for your help.

[Anonymous]

Thank you both for responding. 

From the SVG file, I deleted the interior lines, then I unfixed all the lines. 

I then go to offset the svg files edge x2 to get the lines you see. 

I researched a few plugins to check for gaps in the lines, so far no lines have gaps confirmed x2. 

Any way to get the added exterior lines into the profile? (Orange stuff ;-))

Are Profile planes editable? I have joined them before but had a body to inspect.

[g-andresen]

Hi,

Without watching the file a statement is not possible.
Please upload the file.
With offset of imported contours it comes occasionally to breaks or overlaps.

regards

günther

[davebYYPCU]

After checking the sketch for gaps, stay in Edit Sketch mode, 

Select all the curves, right click, check in that menu for, 

Move to Sketch Plane

if it is in the menu, use it.

Planes - editable, no idea what you mean.

Might help...

[davebYYPCU]

There is a Preference setting for that now.

[Anonymous]

Here is the file I am regarding. (does not let me add)

So far I found a solution. I am pretty sure I have read it in the forums somewhere. 

After I insert the SVG file, I can edit the sketch to offset the lines, etc. Usually, I will need to edit more of the lines to make it easier later to fillet and round edges. 

From there I can open a new document and copy and paste each line and a new Plane is set for the largest image. Note: each line will have to be transferred. 

Worked for me so far today. But I am still curious how the plane can be edited. 

Pic one is the original issue. Pic two is what I am trying to make happen without going through the steps above.