linear step and repeat. 1

[PaulnKY]

Under tools/sketch tools. "There is liner step and repeat".
I am trying to control a hole series at the assembly level and using this command was the only way I have found to array a hole series. The hole array needs to be design table driven but I am having a hard time determining what the parameter name is for this pattern. clicking on the differnet entities gives me the properties for thos entities and not the pattern. Any ideas?

 

[SBaugh]

You can't control a sketch linear and repeat from a Part in an assembly DT. That might be the reason why your having trouble.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[PaulnKY]

The sketch and the hole series are at the assembly level. not the part level.

 

[PaulnKY]

I dont' see any entry in the browser for this feature. The only way I have found to edit it is to edit the sketch, click on one of the points that are part of the pattern and listed with the constraints is an entry called "patterned". by right clicking on that, I can edit the pattern. but I still have not found the name in order to control it from the DT.

 

[SBaugh]

Forgot to add in a sketch linear and repeat your not givin the number of instances and the offset. I think that's the problem your having.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[PaulnKY]

I'm not sure what you mean by "not given the number of instances and the offset". I set the X and Y spacing and the number of entities in each direction. Once set I can edit the number of entities in each direction but not the spacing.

Here is what I did.
I started a new sketch at the assembly level on the face of a part. I put in one point and used linear step and repeat to create an array.

I used "Hole Series" on the hole wizard to create holes that would be visible at the part level. Now if I go into sketch mode and edit the step and repeat, the hole series matches whatever changes I make. This is exactly what I want. But how do you control a linear step and repeat in a DT. I know lots of people here will tell me all this should be controlled at the part level but that would mean I would have to open 30 to 40 parts every time we make one of these. And I do mean one. The next one we do will be different. We NEVER make the exact same thing twice. Assembly geometry needs to drive part geometry. This is how we have to work.

 

[SBaugh]

I was wrong in saying instances. You can only edit the instances. It's a limitation to edit the offset in the X and Y direction.

I started a new assembly, started a sketch on the front plane drew a box. Click Linear pattern in sketching. Give it a distance in X and in Y along with how many. I clicked OK everything is fine. I editted the linear sketch and repeat. I can only make changes to the amount of instances and the distances that I added. This is the limitation I just told you about above.

Why don't you add the series of points to the sketch in your Hole wizard? You could add the points in with some controlling Dimensions and relationships. Then you could control the sketch points with those dimensions and take out the problem of the Linear step and repeat.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

The only way I have found to edit it is to edit the sketch, click on one of the points that are part of the pattern and listed with the constraints is an entry called "patterned". by right clicking on that, I can edit the pattern. but I still have not found the name in order to control it from the DT.

You do not control the pattern directly, you control it by the components of the pattern ... ie; the Offset or Spacing dimension & the Quantity.

1) While (or after) creating the pattern, rename it to something easily recognizable (eg EXAMPLE_PATTERN), then double click on it in the Feature Manager, then RMB on the offset dimension shown in the graphics area, click properties & change the name (from probably D1) to say OFFSET. Then RMB on the quantity (It is sometimes hard to find, but will probaby be at the origin of the original pattern feature) & rename it to QTY.

2) Insert your DT, using the Blank switch, & in the selection box which opens up, select the OFFSET@EXAMPLE_PATTERN & QTY@EXAMPLE_PATTERN & click OK. Your DT should now be populated with the controlling features.

3) Fill in the cells to suit.


from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[PaulnKY]

"1) While (or after) creating the pattern, rename it to something easily recognizable (eg EXAMPLE_PATTERN),"

This is THE problem. How do I rename it? It doesn't appear in the feature manager. It seems to be residing within the sketch. I can edit the sketch, RMB on any of the points I have patterned and edit the pattern that way but I cannot find a way to get the name of the pattern in order to rename it. No dimensions are shown when I edit the pattern.

I need to install the service packs. I'll do that and see if this was addressed.

 

[CorBlimeyLimey]

I don't understand why you are having a problem. What you should see is something like this:-

Explain step by step procedure of how you create assembly hole pattern.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[SBaugh]

This is THE problem. How do I rename it? It doesn't appear in the feature manager. It seems to be residing within the sketch. I can edit the sketch, RMB on any of the points I have patterned and edit the pattern that way but I cannot find a way to get the name of the pattern in order to rename it. No dimensions are shown when I edit the pattern.

That's what I have been trying to tell you Paul. You can't edit these dimensions and you will not be able to add them to a DT. A SP will not fix this. If you have any API skills MAYBE you will be able to extract that information but I cannot guarantee that.

I have however just found a way around this.

1) Edit the "Linear sketch step and Repeat" - NOTE: Edit the Sketch only!! Don't RMB and go in the function.
2) You should see 2 construction lines.
3) Add a Dimension by picking only the Construction line. For each line.

I added the dimension and changed it from 1" to 2" - Editted the the "Linear sketch step and repeat" and the dimension in the greyed out menu box changed form 1" to 2"

4) See example shown here -

http://www.scottjbaugh.com/Linear_Sketch_Step_Repeat

5) Now you can use those Dimensions in your DT.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[PaulnKY]

What you are showing is a Linear pattern which will work with a regular hole. The only hole that can be done at the assembly level that will be there when you open the part file is the hole series on the hole wizard. The standard linear pattern is grayed out when I pick the hole series.


Here is what I did.
At the assembly level, insert a new sketch on the face of a part. put a point in. Under tools/sketch tools, there is linear step and repeat. This will array that point. Exit the sketch and use the hole wizard but pick the hole series tab to make the holes. This will make the holes in the assembly AND at the part level which is what I need.

 

[PaulnKY]

Scott thanks for your patience, nice workaround. But the dimensions between the holes is a constant, I need to change the number of holes in a direction.

Hmmmm . . .

 

[SBaugh]

That doesn't matter, put the dimensions on those Construction lines. I did it with points just now and it works fine.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[SBaugh]

I can send you a AVI file of this if you need it. Give me an email address.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[PaulnKY]

Hey Scott, that will control the dimensions but how does that control the number instances?

 

[SBaugh]

I thought the dimensions is what you wanted?

Again though, like I said in the beginning you can't control this sketch function. Because the menu dimensions and instances are not put into the sketch. So using this function is not going to work for your DT. Unless you know API and can find a way to suck that information out of that menu then there is nothing you can do to add to your DT. I managed to get the dimensions in the sketch for control into a DT. You can't control the instances without RMB and going into that menu function.

You will need to find a different way to build this file. You might try looking into CLB suggestion of using an Actual Linear pattern in the assembly of the Hole Series.

Regards,

Scott Baugh, CSWP

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376

 

[CorBlimeyLimey]

PaulnKY
Try using Equations instead of a DT. An Equation can link pattern dimensions & quantities between parts in an assembly where a DT cannot. eg: QTY@LPATTERN1=QTY@LPATTERN2, OFFSET@LPATTERN3=OFFSET@LPATTERN5

A linear hole pattern could be applied to each of the parts involved & cross-referenced to each other via the Equations. You would then have to edit a couple of equations & update or rebuild the assy.

I have tried it on the simple example I posted above & it worked well. Your situation is probably more complex but hopefully will allow this method.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[Dennyd]

CorBlimeyLimey,

Actually, I prefer to handle a lot of situations in a design table instead of with equations. Since the DT is a spreadsheet I have tremendous latitude for calculations and IF statements. I have one DT with an extra sheet in it that I copied in. The first sheet of the DT is used to control the values for the one or many configs, but it references cells in the second spreadsheet. This is terrific!

I have another DT with a ton of Lego type bricks where I only put in the number of pegs in a row and the number of pegs in a column. The other cells reference these two numbers and determine the number of other instances in their respective patterns, lengths, and even suppression states, i.e., for a 1x1 brick the patterning of the pegs is suppressed. With the right kind of IF statements this is a snap to cover a large set of possibilites. This is much easier than done with equations.

It is great that we have several ways of doing something; manually, equations, design tables, linked values, etc.

- - -Dennyd

 

[CorBlimeyLimey]

Dennyd
I prefer using DTs too, but in this case a DT cannot do what is needed, whereas the Equations can ... maybe?

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.