Linear Sketch vs Linear Pattern

Personally I do not like sketch patterns and recommend our users to stay away from them if they can.

1.) It is sometimes hard to fully define sketch patterns. Especially if you delete the original sketch item from the pattern. It also adds more complexity to the sketch for future modifications.

2.) Feature patterns are much easier to manage. - Easier to modify - You can suppress feature patterns. - Easier (less steps) to remove an instance. - Easier to understand the intent

According to some tests done last year a feature pattern rebuilds faster and create smaller files then a linear sketch step and repeat

Krister L

For many of the previously stated reasons, I vote for the feature pattern. I don't know if it will always rebuild faster than the sketch pattern but I would recommend selecting the "Geometry Pattern Only" option whenever possible.

JJ

Matt Lombard has this written down in his Rules of Thumb.....there You can compare file size and rebuild times for different kinds of patterns.

Krister L

I was going to inquire about that. Thanks.

An advantage of feature patterns may not be apparent at first. Just this morning one of our guys here had created his base extrude with several holes in it. (Ok, fine, stuck ACAD user, he'll learn.) But then he put in some Hole Wizard tapped holes, patterns, etc. Now, today he wants to remove one of the original holes in the extrude sketch. Upon editing that sketch and deleting the circle, apparently the base extrude rebuilds with a different ID, as the child features don't like it anymore. No sketch relations at all to the circle in question, just a circle in the sketch. Remove it and other things fail.

So, the moral of the story is that features are easier to manage later when changes are implemented.

WT

Could one way of solving a problem like that be to simply pick the cylindrical face of the hole in and select "delete face" instead of editing the sketch.?....But I'll also put the feature patterns before the sketch ditto though

Krister L

I just tried a test part on what I described here about taking a circle out of the base extrude, and it worked just fine. He must have had something else goofy in there that we didn't find. Sorry. :-|

WT

feature patterns are very effecient when populating assemblies with fasteners

One problem with patterns inside sketches is that you can not add entities to the pattern once the pattern is made.

Hopefully you can benefit from my painful experience. I just finished a part. A hat channel 90" long with 58 pairs of hooks to be punched out from the inside of the hat. (And two other configs with short length and fewer hooks.) The hooks were 90 degrees down and 85 degrees up. I spent long hours getting it "right".

Initially, I cut the outline (material removed by the punch) I "knew" enough to use symetry so that my my Extrude-Thin1 was half the part. I made it sheet metal and rolled back to make the cut. The first outline cut was patterned the 58 instances. Then I mirrored. So far so good.

In my ignorance, I edited the Flat-Sketch1 in Process-Bends1 to make the bends for the hook. (I had a another part with a modeled by another to go by. This was how he did it.) I In the Flat-Bend1 sketch I again used symetry by first sketching a centerline to use two lines across the pre-bent hook area. I then did a step and repeat for 58 instances. A step and repeat in one direction needs a dimension manually added between one step and another to constrain the pattern. (You would think Solidworks would do the dimension for you because it knows you only went one direction)

Imagine waiting for that rebuild only to find that the 116 hooks were pointing the wrong way. I was able to determine that I could select and edit the bends to make the second bend opposite to get them to point "right". Each Sketch bend had to be edited by itself. I needed to do 116 of them! each rebuild took about 7 minutes. 7 x 116 = 812 minutes. 812 minutes/60 = 13.53 Hours! After 5 hooks I realised i had nother problem. How was I going to make the other bends not 90, but 85 degrees! Not counting the time it would take to figure out how to do that, my task would take 27 hours! It was time to call my VAR for help.

He explained I should make it two individual "Sketched Bends" Using SolidWorks Help this was simple. This gave me the hooks with the proper direction and angle without having to manually edit each one. But, I know had two features with linear step and repeats in them. Rebuilds still were irratating.

At this point, managment forced me to send the drawing off to the vendor to get the punch tooling ordered. This was before I knew if the hooks would be strong enough. Off the files went. I made a smaller version of the hat channel to run CosmosExpress. I was pleasantly surpised with margin of safety.

I called the vendor this morning to see how he liked my rebuld time. He said he spent a hole day making his shop drawing. He made a couple of passes with Pallet Forming tools. The first one made the outline and the hook and the second made the hook and then he cut the outline after. Both versions of course eliminate the linear sketch and repeats, replacing them with a sing feature linear pattern. I asked him for the forming tool he used.

He sent me both explaining he used the second because it was closer to my model. He could make neither exacthy the same as mine because of the minimum radius limitation when modeling the forming tool (another subject).

I made a new configuration of my part and did the form and then the cut. Rebuilds are now seconds instead of minutes. He called asked how I did. Of course I was very thankful. I told him we could both use the quicker of the two because the tool was made per my original. If my hook design doesn't prove out I have to buy new tool anyway.

A really big payoff will follow whan I make the configurations of the shorter versions. I would have to supress the Sketched-Bends made for the 90", and make new Sketched-Bends for each new config because you can't change the step and repeats.

Now the downside. Had I gone the feature pattern up front my FEA results would have been different. Maybe time consumingly different. Both forming tools produced an ugly mess of surfaces exactly where the highest stress was. I haven't done the FEA on the "new" hook but I know the results will not be the same. I may have had sleepless nights.

I have to admit I chose the sketch linear step and repeats because of my lack of success making forming tools, and the management pressure. (I'm self taught user with little training. This ng helps a lot. Through it, (Paul Salvador's link) I knew of the Lombard Rule uf Thumb for this was. Thanks all.) and was hoping in advance for the help I received from the vendor. He is a much better modeler than I am. Design was more important. I'm convinced things worked out the best they could. The linear step and repeat produced a model closest to the real world for tooling and FEA, and the feature linear pattern gives much better productivity now.

I hope this helps.

Actually You can....easily.....highlight one of the patterned entities ...it shows up in the property manager like "PatternedX"....rmb that one and select edit pattern....now You can increase or decrease the number of entities Or...rmb one of the patterned entities ...and select "Edit Linear Step and Repeat If You wanna change the distance between the entities, just put in a dimension and adjust it...same goes for angles

Krister L

I am curious to see the part - would you please send me a copy.

WT

Sorry...language confusion...after reading again I see what You mean....and yes You're right ...You can't add more entities

Kriste

Yep I tried it too. I was very surprised that you could not add another entity. This goes back to my first post on this topic where I stated that I recommend, to our users, that they stay away from sketch step and repeat patterns if they can.

mean....and