Covering tips, tricks, workarounds (grrr) & strategies from the viewpoint of a general user of Inventor and Vault (and some associated products & off topic subjects). Feel free to comment as you see fit. Just keep it real & relevant :-)
In the above picture I have used only 1 sketch for the locations of the slots and the hole. I created the Cut feature for the slot first and then shared the sketch so that I could add a Hole feature.
I hit a snag when I started the Hole feature in that both of the Sketch points were chosen and I couldn't un-select the point in the middle of the slot. I tried Shift and click and Ctrl and click, nothing worked.
The solution was to exit the Hole feature, select the 1 Sketch point first and then start the Hole feature again. This limited the Centres to only the 1 I had chosen and I was able to complete the Hole feature.
Below is a quick video of the process, and me stuffing the Hole direction up which I promptly fixed. No comments needed on that, we are all human (just some more human than others).
While writing this post I realised that it's practically 1 year to the day since my last post! Seems like only last month. Time sure flies.
Anyway, onto the topic of this post. The title is really referring to Structural Steel members placed from the Content Centre (CC). Each family, even those supplied by Autodesk, appears to be an extrusion from the Start Plane out 1 direction, therefore making a midpoint Flush/Flush constraint difficult because you need to do some calculations (1/2 the member length) to get it constrained mid-plane into your assembly. For reasons I won't go deeply into now, I place all CC members as Custom. I do this is mainly because the file becomes somewhat editable and I can change the extrusion to get the mid-plane where I want it, in the middle.
Work is biting into my post schedule so this is just a quickie that I discovered myself just today. The context is that I want to pattern the 2 diam 14 holes at the top (12 o'clock) 3 times meaning that I will have a set at 3 and 9 o'clock. Because I started at 12 I can't get that pattern without doing it 4 times in 360 degrees and then RMB on the 2 holes I don't want and Suppressing them.
My discovery today is the double arrow in the bottom right corner of the Pattern window. Expanding it shows a Suppress button and if I hit that and select either of the 2 unwanted holes the command will Suppress those while inside the Pattern command. A real time saver which in my books is a bonus!
Below is a video of the process. Note that this is in 2014 so I expect it to also be in newer versions, but whether in older I don't know.
I greet you with a short post due to work commitments. The post is about the variety of PDF file sizes I get with the 3 programs I use. This is something I've noticed for a while and it's become more critical since I upgraded to mobile broadband (from dialup - yuck) and I now have a strict quota with big $ overtime charges. Why I'm on mobile broadband is a long story which I won't go into, except to say that landline broadband isn't available at my bush block 'little patch of heaven'.
My PDF writer of choice has always been CutePDF due to it's small size, easy configuration, great output and community support. It is just a great and simple tool to pump out a quick PDF. Next was PDFCreator which is no where near as simple to use or configure, and conversely is powerful in it;s batch ability and many other attributes which I often use. Finally, and only if I had too, I would revert to Inventors built in PDF Export which feels clunky like Inventors Print Dialogue, and for this reason I didn't use it.
The picture below shows the various file sizes created by each of the programs. I have to admit that I'm surprised by Inventors Export PDF file size which is the smallest by a long way at 462 KB.
I did a few tests with CutePDF, trying to see if I could get better results and I could only get the file size down to 2.41 MB which is only a small decrease from the default settings which produced a 2.64 MB file. A quick Google search showed my how to change the dPDFSETTINGS value in the config file and I tried each of the options that should create a smaller file, but I experienced only a small change.
PDFCreator had a better output than CutePDF but still a long way short of Inventors output. PDFCreator produced a 1.76 MB file with a bit of tinkering.
The same Inventor IDW file was used for each of the tests, and each PDF printer was set at 150 odd DPI and full colour and A3 size. There was no noticeable difference in any of the PDF files.
So, with some humble pie swallowed I'll have to start using Inventors Export PDF a bit more. I just need to find a way of locking in the DPI at 150 because it annoyingly keeps changing back to 400 DPI which will again blow the file size out, and from a Print Range of All Sheets to Current Sheet which is just a royal PITA, and to stop the PDF from automatically opening. Not asking for too much, hey?
Now, if I could just find a person smarter than me (shouldn't be hard) to write me some iLogic to run the Inventor Export PDF with All Sheets on and 150 dpi I'd be as happy as a slinky on an escalator :)
This week I've taken on some home based design/drafting for my day job employer. Getting the templates is easy as is the Design Data, but 1 thing I struggled with was the custom Content Centre (CC). At my day job I have heavily customised the CC to suit our requirements. I have added a lot of content based on custom rolled profiles we make and to make up for the basic amount of Australian Standard (AS) data that comes with Inventor. Through my day job VAR I found that the good folk at Autodesk made a method to allow me to export this custom CC and to bring that into my home Inventor so that I can work with the custom CC data and expanded AS families. In this posting I'll only be showing how to get a Vault CC Library exported for Desktop Content, but the reverse is also possible through the same set of dialogue boxes.
Recently I stumbled onto a very annoying bug and regardless of many methods to get around it I couldn't. It's simple enough to replicate. It just requires me to create a sheetmetal part and a cone with an included angle of more than 60 degrees. Then use the Unfold command and refold (using the same stationary reference) and the refolded part is truncated and offset from the original cone model and UCS. But there is a simple enough solution (workaround) that's not immediately obvious.
It's been a long while since I last blogged, and I have really missed it. Blogging doesn't pay the bills so it takes a back seat to paying work.
Recently I had a need to place an aligned dimension between 2 holes, but whatever actions I took I couldn't get quite what I wanted. I eventually settled on rotating a Detail View and placing a standard horizontal dimension, which I can use but don't really like. I posted this to the Inventor forums and got several responses all of which are acceptable (some more than others) and I also posted this to the IdeaStation where I got further valuable input.
In this blog entry I will gather together what I have learned in the last few days about this seemingly easy requirement and the cons and pros of each method.
Method 1 - rotate a Detail View
This method is simply to create a Detail View of the area of parts you want to dimensions and then RMB on the Detail and click Rotate. Then use the rather intuitive controls to make it horizontal/vertical and then place the dimension. I finish this by adding a note to the Detail View label that the view is shown rotated. A video is posted below showing this method.
Pros - easy, placed dimension is clear, the view can be rotated again and the dimension sticks (I didn't show this in the video but it works).
Cons - not entirely intuitive to the drawing reader, requires quite a bit of work.
Method 2 - create a view sketch
This method uses a sketch on the view to create lines that the aligned dimension can be created with To start I single click the view and then select Sketch from the ribbon. Then I projected the 2 circles and the edge for dimension alignment. It's not strictly necessary to project but I do anyway. Then I created 2 connected lines, the first starting at the centre of 1 circle and the second ending at the centre of the other circle. Then I made a aligned constrain between 1 line and the projected edge I want the dimension parallel with and then a second constraint of perpendicular between the 2 sketched lines. Finally I turn 1 of the 2 sketched lines to "Sketch Only" type. I then exit the sketch and use the remaining line as the start of the dimension and the centre of the other circle as the end. A video is posted below showing this method. This method was suggested by admaiora.
Pros - relatively easy, rotation changes to the view stick.
Cons - not intuitive, requires quite a bit of work, not easily visible in the model tree.
Method 3 - chain dimension
This method uses the Chain Set dimension tools. I start by issuing the Chain Set dimension command and then select the line I want the set aligned to. Then I continue selecting the 2 holes and then RMB and select Continue to then place the dimensions. After exiting the command I then RMB on the dimension on the end and select Delete Member. I repeat this for the other unwanted dimension and am left with the dimension between the holes. A video is posted below showing this method. This method was suggested by mpatchus.
Pros - relatively easy, rotation changes to the view stick.
Cons - intuitive to regular sketch users, requires quite a bit of work, some variable results (not shown in the video but they were experienced).
Method 4 - rotated hole centre marks
This method uses the ability to rotate hole centre marks so that 1 is aligned with the direction I want the dimension at. I start by placing standard hole centre marks and then I RMB on one of then and select . A video is posted below showing this method. This method was suggested by Doug_DuPont and jletcher.
Pros - easy and intuitive.
Cons - some users/companies require centre marks to be horizontal/vertical aligned so extra commands needed to re-rotate the altered centre mark.
Method 5- centre line through tab
This method is similar to method 4. It uses a centre line through the tab near the largest hole as the basis of a dimension. A video is posted below showing this method. This method was suggested by jletcher.
Pros - easy and intuitive.
Cons - in my example this is applicable but if no tab is available or the hole is not in the middle of the tab then this method is impractical. Deleting the centre line also removes the dimension. Leaves an ugly and unwanted centre line.
Round Up
While all of the above methods have their use I feel that most miss the mark. Out of the 5 methods number 4 holds the most promise as it is intuitive, easy to implement and looks good. However I feel that there is still something missing from Inventor in relation to an aligned dimension. Thinking back to AutoCAD I could create an aligned UCS (aligned with a line) and then place the dimension and then return the UCS to world. While I'm not after this exact workflow in Inventor I feel that starting a dimension, clicking the 2 points and then a RMB and select something like Edge Align and then pick an edge is a better and even more intuitive method than that detailed in Method 4.
Feel free to make comments and suggestions. Maybe I (and the helpful forum posters) have overlooked another even better method. And many thanks to the forum posters for their help.
Footnote :- I apologise for the video window size and quality, some of which is out of my control. I'm still learning :)
