Freezing when working with patterned sketches

[Anonymous]

Hi,
I have created surfaces then a body from a sketch - (screenshot "A") attached. I am having several issues when working with this and other repeated patterns when the sketch increases in size. When working with the same pattern in a smaller size, there's no issue. So I am wondering if I could get some advice with an approach to making these grid patterns (I have many to make).

The scope of work I need to complete is to create several very precise grill elements (eg. the one in the screenshot) to use as cutting tools for other bodies. I will be making similar patterns in hexagons, octagons etc. The circle size in this case is 11.5mm, the thickness of the tubes is 0.3mm and the top edges are filleted to give a rounded edge.

Methods tried to achieve this tried so far are:
A
1. Created a sketch (Screenshot "B")
2. Went into Patch mode to extrude the lines into surfaces
3. Then thickened surfaces to create bodies
4. Then combined these bodies to make body (A)
5. Applied a rule fillet to the top edges
6. I then realised I needed to increase the extent of the sketch so decided to add more circles and pattern around the center as it was taking a long time to draw (Screenshot "C")
7. Repeated steps 2 to 5 to create another new body (B) to join to the existing body created
8. Tried to combine body (A) & (B)

B
1. Created a portion of the sketch
2. Went into Patch mode to extrude the lines into surfaces
3. Then thickened surfaces to create bodies
4. Then combined these bodies
5. Applied a rule fillet to the top edges
6. Patterned these bodies around the center
7. Then combined these bodies

Problems encountered:

When increasing the size of this type of sketches (many shapes of the same size joined together to form grids), Fusion 360 slows down dramatically or freezes. Is this normal?

Copying and pasting sketches of this size/ nature regularly causes Fusion to freeze. How can I do this without this happening?

When trying to thicken the surfaces I could only select 7 tube bodies at a time as Fusion would freeze if I selected any more. Is there a quicker way or a work around for this to speed up the workflow?

When trying to rule fillet the surfaces Fusion would freeze ,possibly due to the size of the body? Is there limits to the size of rule filleting one can apply?

Could not combine body (A) & (B) even though after much checking, geometry was perfect. Why would this be? Can you suggest something to do when this occurs? Makes no sense when the geometry is so accurate?

I tried creating more than one sketch to extrude, thicken, combine etc to achieve the same result to overcome the issue of fusion crashing due to the increase in the size of my sketches.

This is a very brief overview of what I encountered during a long and frustrating day. I have had the same problems in the past for grid type sketches on Fusion and I really would like to know a method of approach which, Fusion 360 can cope with in creating these type of grid bodies. Can anyone suggest the best way to go about this?

Many thanks,

Tony

[innovatenate]

What is the intent of the work? Are you going ot manufacturing this "grated" portion of the design? If not, you could create a custom appearance with "cutouts" to apply a simple solid. This will give you the appearance without requiring the computational overhead of creating all of the goemetry. 

Does that help?

Thanks,

[Anonymous]

Hi Nathan,

Thanks for the reply. I am trying to create several grated extruded structures to save and use as cutting template tools for patterning surfaces in other bodies (to create effects equivalent to Jewelry embossing, engraving or stamping and sometimes cutting right through.) I am designing geometric based Jewelry. These grated template bodies are then to be scaled and used for many other projects I have which require such patterns embossed on faces. I had a look at the video you attached and require further investigation/familiarity to see if the cutout method is something that can achieve the results I'm looking for. With this information I've provided, do you recommend pursuing this method?

Kind regards,

Tony

[innovatenate]

The difficult part about this type of question is that there is a geometry ceiling that every CAD software will run into. 

In the case where you are manufacturing the geometry, this work-around will not help most likely. As an example if you were designing a grated walkway, the expanded metal used for the floor of the walkway would be a purchased item. Since you would not be manufacturing these components, you could get away with this appearance approach. Since I suspect you will need to create a DXF for a (cutting/engraving) path, or to create a toolpath in CAM, or 3D print this solution may not help.

I would be interested to hear more about the manufacturing process. I'm not totally sure how the jewelry is going to me manufactured (by hand, by machine) or if it is necessary to have the geometry in the model. Are you just looking to generate renderings to show off concepts or is will a computer aided manufacturing 

I'd also like to mention that there are other solutions like this image to surface add-in on the Fusion 360 Github site.

https://github.com/hanskellner/Fusion360Image2Surface

In this case where you need a DXF and you would like to do a pattern, my advice to achieve successful geometry creation with the best performance follows:

• Pattern 3D geometry, not sketches (it will be faster to compute the pattern). If you can find the the minimum viable sketch base to pattern, create that. Something like the below image should work

• Fusion 360 provides several different options when patterning 3D geometry, Face, Bodies, Features and components. Features are the most unpredictable option since features can have dependencies (e.g. patterning a fillet requires an edge to be referenced). However, it does have an option for Optimized calculation. I believe that patterning faces will be faster than patterning bodies. I've attached a couple of sample approaches below for you to review. 
• Last, once the geometry is complete, you may be able to use the command Sketch > Project/Include > Intersection command to generate a sketch from the 3D geometry. You can then use this sketch to export a DXF for engraving or laser cutting, etc.. 

This is by no means the absolute answer, but I hope some of this information will help get you where you need to be. Let me know if you have any other questions or concerns.

[innovatenate]

I just thought of one more thing that may impact performance. There is Direct Modeling and Parametric Modeling Environments (timeline), you can read about how to switch the environments in the below link.

https://knowledge.autodesk.com/support/fusion-360/troubleshooting/caas/sfdcarticles/sfdcarticles/How...

Working in Direct Modeling may give you some performance benefits, but you will lose the parametric (timeline/history). 

I hope that helps. 

Thanks,

[Anonymous]

Hi Nathan,

I'm so appreciative of  your detailed answer, this has helped me a lot in terms of direction and options to try.

 FYI The grated cutting tools would be used to cut out the patterns on flat surfaces around 0.2 -0.3 mm depth of cut upon 1mm thick bodies. The manufacturing process would then be 3d printing, molding and casting.

I'm off to try out all the solutions you came up with Nathan!

Best wishes and thanks again

Tony