Inventor TP: Edit Hose connection

Last weeks post really as some of you might see it on Autodesk forum but my intention to improve and expand on the subject has pushed it couple of days forward and no extra info sorry to say and It feels that if I don't do it now I will never get round to do it.

Question cam from my old friend +Alex Fielder about editing hoses that don't update with the moving equipment. One day he came back to his project to realize that all of his hoses were floating around as if they lost the connection point. 

I did remember that -niels- on the Autodesk Forum has mentioned this happening to him and his problem was due to the fact that he had opened the assembly in express mode without realizing and it all wen't crazy until he load it in full and did a "rebuild all".

I had this problem with fittings not moving with the equipment and the only solution then was to edit fitting connection, delete the connection then connect fitting again. I alwasy constrain the T&P assembly and all the runs inside but I suspect that in this case I have grounded the T&P assembly wihtout realizing and that might have been the problem.

Now back to our question: Are we talking about a hydraulic hose with fittings our without? Slightly different approaches here.

I will describe a hose without fittings procedure because it includes the one with fittings.

1 - Edit the Hose route and change it to Hose with fittings (your choice of fittings).

2 - Finish and populate the hose run.

3 - Edit the Flexible Hose assembly ( assembly that contains the hose route, hose fittings and hose part)

4 - Right click on the fitting you need moving (the one not updating for you), choose edit fitting connection and remove the connection that you wish to move, update or relocate.

5 - Delete the connection, keep the one on the hose and click OK.

6 - Step up at the run level that contains this flexible house assembly. And use the “connect fitting” command. This will be unavailable/greyed out at the flexible hose assembly level. Select the end of the fitting and the location you want it moved to.

7 - Go back inside hose route and change the style to hydraulic hose no fittings and finish the route.

You need to change style to hose with fittings because otherwise it acts as a route continuation rather than moving the end connection point.

Later,

ADS

Compare drawing sheets

We had this weird problem the other day and deciding to investigate some more resulted in this post being created because it seemed helpful.

                Looking through our Vault I found one drawing that had not been dated and approved. So I open the drawing with AutoCAD and to my surprise it was signed and dated. I double checked on the physical copy that we file and confirmed that it has been singed and approved.

                Somehow in the publish process AutoCAD has messed up the dwf so Vault preview image would not see this changes. Not knowing what else might have been omitted I decided to compare the drawings and for speed and accuracy I choose to let the computer do this while I, like a good manager I am, supervised the process!

                The only way to compare files was trough Design Review so hit right click in vault on the drawing preview image and select “Open in Autodesk Design Review”. We are now ready to compare and it can only be done against other dwf/dwfx files.

                Open the drawing in AutoCAD and exported the file to dwf then I was able to use the Compare Sheets command in Design Review.

                By default any addition will be shown in green and deletion in red but you can change those colors if you want in the Options part of the Open window dialog.

                Luckily that was the only difference and after checking the drawing back in it all updated. You don’t need to use check out/in and you can just click on Update View in Vault to make it current.

Later,

ADS.

                 

Inventor Assembly Template

                There is a lot of info on the internet on how to setup your template files and many of you have already configured the drawing template, adding title blocks, borders and some symbols maybe. You have probably edited the part template and changed the default material but chances are that you haven’t altered your assembly template too much if at all.

                I am saying this because I see recurring questions popping out every once in while by frustrated people doing repetitive tasks that could have been avoided with a proper setup of their assembly template.

                One of the main things that will save a lot of frustration would be to setup a new design view representation as default instead of the locked “Master”. God knows how many times I’ve found Assemblies that cannot be saved because of the “Main design view is locked” error.

TIP: Instead of locating the template file and folder you can create a new file using New command and then save those changes in the template using Inventor (big I top left) / Save As / Save Copy As Template command.

                So open your standard.iam file template or fire up the new assembly command. Create a new design view representation, I call mine “Default” and set is as active. This will become the default view and hopefully if you don’t manually change it back to Master you should get over that pesky error on editing locked design views.

                The next one up is BOM. By default the Structured tab is disabled and every time you place a Parts List or edit the BOM you need to activate it. You then set it to All Levels, you may change the default delimiter and most certainly you will add and remove columns to suit your design needs.

So why don’t you go ahead and make these changes persistent in the template?

Depending on your design process and needs you might not use this but I recommend that you add Item QTY to your BOM. This will report the cumulated number of instances in the BOM. The default QTY will report the number of items as long as the item doesn’t have a length (G_L parameter) like structural sections, pipes, etc. in which case it will report cumulated length and not the number of items in the assembly.

                I feel better already, anything else?

                I use a lot of Content Center and Purchase Parts that are library read-only items and when doing large assemblies it’s hard to navigate the browser to find that part you want to edit. So what I like to do is add two folders called CC (Content Center) and PP (Purchased Parts) where I group the files to clean up the browser keeping just the normal parts. It makes a huge difference to be able to find something fast not to hunt and pick all the time. Also, you can now suppress hide or disable a whole folder at a time ;)

                Nice... what else?

                How about adding some virtual parts? This is where you get creative and to utilise the tip above you might want to add them to a folder called Virtual. It’s better to add as much you can think off and then delete them in the assembly later if not used. Creative? Like what? Stuff like oil, grease, man hour costs, machining costs, shipment, painting, etc. Remember that you have Estimated Cost on iproperties and virtual parts although exist in the assembly only they do have iproperties just like any other parts. You can even add a long descriptive text in the comments field. Do you need to add the Estimated Cost to BOM? How about Comments then?

                Keep going please!

                 Anything you need changing in the Document Settings? Maybe you want to change the default Lightning Style, maybe not but you might want to change the default dimension display to “Display as expression” to see the full equation driving that dimension. In here you can change the units as well as modelling precision. Verify all the tabs and make sure there’s nothing else that needs changing.

                Is this it?

                On the short list you might also consider:

·         Deactivating the Contact Solver in Inspect Tab

·         Parameters that you keep adding all the time like bounding box dimensions.

·         Link or embed some excel files

·         Add various iLogic Forms if needed

·         Add some iLogic code like one to prompt you to fill in iProperties at first save.

·         Turn on Center of Gravity

·         Etc.

I suggest that every time you find yourself changing settings in an assembly pause and think if this is something that might be saved in the template. If you do this for a week then you’ve probably got most of things but it’s a good exercise to do every once in a while especially with each new Inventor release.

               

Later,

ADS.

Drawing curves to match model

HOW TO SET DRAWING LINE COLORS AS MODEL APPEARANCE?

I wasn’t sure if to post this at all because it didn’t seem to provide any good and positive solution. If at all I would have post it under “food for thought" or under “let’s see if we can find a better solution”. By “we” I mean one of you showing me how to properly do it.

But just the other day this showed up as a question on the forum and seeing that none came with a better-closer solution I decided to share it as a full blog. It doesn’t mean that you cannot correct me, in fact I am hoping one of you will do.

After posting my answer  the guys on the forum went quiet so I take it that either my info was more than they expected (yeah right!) or I am so far out that they are embarrassed to tell me. I think it’s the later, I’ve been there more than dozen times.

Before I continue here is the forum post.

             

Following text is an expanded adaptation of the answer provided there.

I've been playing with this on my last project. Because it was a large assembly and the pipes in the drawing ended up looking like steaming spaghetti I decided to show each run with a different colour matching the appearance set in the model.

I did a brief scan on the net to see what others have done and I got excited, almost making me think it was done before. So it was, just not the way I needed because the solutions were getting the colour of the part and I needed the colour of the run that is an assembly and the solutions are processing the curves ONE AT A TIME which it’s like watching a painting being done in real time…… a really large one…..with a small brush.

There are not many options here but if it’s a small assembly or just a part that you need processing then presto get the VB or iLogic codes bellow and get them running.

Just like my solution these need a manual update. Now, imagine that I had to add and remove views, sheets, sections, change appearances, change design views, etc. How many paintings can you watch being done in a day? That’s why I have a camera, a fast point and shoot type as well!

First solution: 

Brian Ekins has aVB code but it's processing all lines (curves) one at time and that takes forever. It creates layers with each colour but unfortunately the layers are called as the RBG code of the colour (very hard to identify and edit)

Another solutionon the mCAD forum:

Third solution was on the Inventor forum:

In my case these didn't work because I had a large assembly. This is just one sheet out of six and quite a simple one.

You can change your selection to part filter select your component (or select it in the browser) and then right click properties to change it's colour (override).

This is a partial solution because it's hard to select parts and manually update them all the time (as the assembly changes). But it’s a fast one, almost instant and it changes all line type (hidden, visible, tangent, etc.)

Because I only had visible and tangent lines (small to an ignore number) I decided to setup layers to which I would assign my runs.

So I end up creating copies of Visible layer calling them Run1, Run2, etc. and changed the colour of each one as per the assembly (manual unfortunately).Then right click on a part (or assembly in my case) in the browser, choose "select as edges" and then in the Annotate tab, Format, Layer, choose the layer you previously created.

Hey that’s pretty cool! Or not, because you need to do it for each sheet. You can expand the views in the browser and select a model (my run) in all the views before using select as edges but still to many manual operations. At least once done you can just change the colour of the layer and all sheets update.

Side Note:

Haven't tested but this seems to affect performance and increase the drawing file size. My drawing now has around 50 MB.

So now what?

Will try and put a nice ilogic together to process your browser selection to change its colour from the model on all sheets as per the appearance of your selected object.

This should not process the drawing curve-by-curve. We only have one life. It needs to get the collection of curves and change properties (override) all at the same time. Somehow that’s what using the properties on a model or using the select as edges does. Surely it can be done with iLogic or VB.

Great stuff! When can we have the code?

As soon as I have it, but the way things are going with work overload and no extra time … I might never get to do it.

Later,

ADS.