1. Home
  2. Solidworks CAD Design software
  3. 2006,sp2_section lines

2006,sp2_section lines

I just did my first mold design with the latest release. I have it loaded on my notebook computer for evaluation and decided to use it with a fairly simple design before loading onto my workstation.

Here is why I may hold off:

The way I do a drawing for a mold design is different from what many of you do for regular drawings. A basic 4-view drawing of a mold is as follows:

plan view of b-side plan view of a-side

section a-a section b-b cut in x-direction cut in y-direction (rotated 270°)

The 2 plan views are of configurations that I make for the a & b sides of the tool. The section views are of the total (default) configuration. This is done by putting a default configuration on the drawing, but up off the viewable area. I cut the section through this view and then hide it.

Then to show where the section cuts are, I need to re-create the section lines in the b-side plan view. This is technically incorrect, but follows a long-standing convention specific to mold design. In previous versions we made the sections first with: Insert,MakeSectionLine, then we would create the section view. When making my duplicate section labels, I have always been able to make the section line and rename it to whatever I want. SW would always ask if it's OK to create a duplicate section label, but I would just click `OK' and I would have what I wanted. I would not actually make a section view with those section labels.

Here is the problem with the latest release. Some genius decided to streamline the section creation process and have us skip the `Insert,Sectionline' business. This works fine for making the section view itself. However, what it means for my duplicate label is I need to actually create a view that I don't want and then hide it. I am still allowed to use a duplicate name for it.

I wold be interested to see if anybody else sees this as a problem. Also, I am willing to change to a better way of doing all of this as long as I get the identical result on my end drawing.

Sorry for the long post. Thanks.

jk

Reply to
John Kreutzberger
Loading thread data ...

I also design molds in SW and use the same drawing layouts like you (plan views and section views). The first couple of designs I did, I did like you and hid the view that created the actual sections. But the last two I have done I showed it in the corner of the drawing. It created some confusion at first, but it was easier that recreating the section lines and then having to move them if I changed the real section line. At my work, they were used to 2-d drawings untill I came on board a year ago, and moved the entire company to 3-d. I figured that the change was a neccessary evil of moving to 3-d. If you choose to keep doing it the current way I would suggest just sketching a line mimicking the section line, changing the line font, then placing a note at either end of the line showing the section label.

Reply to
SoCalMike

Hi Mike,

That's not a bad idea. One thing I do to make it easier to re-create the section lines is create a sketch in the assembly right before making the drawing that shows where I am going to create my sections. Then I just need to convert entities in the drawing for my section lines and then hide the sketch in the drawing views.

I suppose I can create blocks for the ends of the lines.

Thanks for the suggestion. We both need to quit working on Christmas Eve...................

Have a Merry One!

jk

Reply to
John Kreutzberger

John,

I'm not seeing the problem that your seeing. For the Fake section line I convert the assembly sketch to the drawing view, select the converted entites, and use, from the pulldown menu, Insert -> section line. For the real section view I sjust use the section icon on the toolbar which creates the section line and the section view. I also tested creating the section line first and then creating a view from the section line and that still works also.

Here's a seperete question for you. I tried a mold design on 2006sp0 and I ran into a lot of problems with external references being lost. The problem only appeared with base parts. Did you run into any problems of external references being lost or mates being lost?

Roland

Reply to
Roland

I didn't start my testing until sp2. I have had absolutely no problems with references or mates being lost. (OTOH, I started with a very simple MUD unit. I have not used any base parts yet.) I was really happy with the modeling side of things with the new release. Didn't see any glitches until I went to make my drawing. One thing to be aware of is that sp2.0 uses the Bluebeam pdf maker. sp2.1 uses a plug-in from Adobe. I have seen numerous complaints about this in the DiscussionForum on the SW website.

I am starting another one today in 06,sp2.0. Don't know if I'll have occasion to use base parts on this one. I'll let you know.

jk

Reply to
John Kreutzberger

Hmmm, My sw2006 SP2.0 installation has the Insert, make section line command from the pulldown menus.

Reply to
Roland

OK, you are correct. I didn't see it originally. (obviously since I went to the trouble to even bring this up.)

If I customize the Insert menu, then I have the option to select the `make section line' option. I could have sworn that I tried this before and didn't see it, but it's definitely there-just needs to be added to the menu manually.

Thanks for helping me through my brain fart. I'll bang on the new release for the rest of the week and see if I find anything else before loading onto my workstation. I'll pay attention to the base part issue you brought up earlier because I use this a lot in many of my designs.

Thanks again.

jk

Reply to
John Kreutzberger

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.