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How do I create a reverse model of a part


DSHAW

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I need assistance to create an impression of a part like making a Mold cavity. For example after I load a part model into IronCad how do I extract some surfaces to create a new block with the reverse image of the surfaces. Or look at it this way, we import a part file...we have to sit this part in a new Block, like a check fixture. How do I copy the parts surfaces into a new block form to create like a "nest". I cannot find one video online to assist with this function. Some high end software packages have what they call is a Mold Split option. You take a part and split it in half like creating a mold around the part? Any advice would be appreciated.

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IRONCAD doesn't have automated mold tools for this function, but it can be done using structured parts. It can also maintain associations with the "part". I'll prepare a simple video to demonstrate the principle along with simple sample part, core and cavity files.

 

Malcolm

Edited by Malcolm Crowe
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Attached is a video of 4 associative IC files (all structured parts).

 

1. The Part. This must be a structured part, so that the "body" can be saved as an associative BREP.

2. Cavity and Core Generation. This starts with the associative BREP of the above part. With this as the starting point we add the various surface and solid bodies we need to generate the "bodies" of our cavity and core. These bodies can then be saved as associative BREPs.

3. Core Mould Half. This starts with the associative BREP of the above single core body.

4. Cavity Mould Half. This starts with the associative BREP of the above single cavity body. I have developed this further with multiple cavities to demonstrate how you can build on the original BREP.

 

As long as these parts retain the same names and locations they will retain their associations. I am not aware of any way to rename or redirect these associative links to bodies. As a result, the sample ICS files that I have also attached won't be associative. However, they may help you understand their construction.

 

I hope this helps point you in the right direction. In case you don't know, to create a new associative part based on the "body" of another structured part, right click on the "body" in question and it will give you the option to save as an external associative part.

 

Malcolm

IRONCAD_2017_PU1.1___Sample_Mould_Cavity_and_Core_Generation.mp4

SAMPLE_MOULD_CAVITY.zip

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Malcolm and IK thank you for the response. I am struggling to see exactly what your doing in the video. This is really important for me to figure out. There's a couple of suggestions here I'll try. Appreciate your patience. May require more help. I tried to open the files and I cannot. You have a newer version. Hum, we pay for updates??

Edited by DSHAW
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Just to be sure, does the principle of what I demonstrated in the video, represent what you want to achieve? That is, to be able to create associative mould cavity and core parts based on the finished product? I don't what to steer you in the wrong direction.

 

From a feature perspective I started using these "old school" SOLIDWORKS techniques in IRONCAD 2012. So unless your version is older than that, you can achieve what I demonstrated in the video. Later versions however include better surfacing tools that are helpful.

 

Hopefully others will be able to share/suggest alternative techniques also.

 

Malcolm

Edited by Malcolm Crowe
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Attached is a second video demonstrating the "steps" to generating mould core and cavity parts. These steps are as follows:

 

1. In "Structured Part" mode start with a linked BREP of the finished part. Be sure to set this structured part to "Active" to be able to add new features to it.

2. Extract Inside Surfaces of the Part using the Extract Surface tool.

3. Using the Patch tool, patch holes where Mould Core and Cavity faces will meet.

4. Create Parting Surface along the desired parting line. In this example is is a simple ruled surface.

5. Trim Parting Surface where Core Body will be.

6. Combine the Parting Surfaces above using the Sew tool, to create a single Inside Parting Surface (for core generation).

7. Repeat steps 2 - 6 above to create a single Outside Parting Surface (for cavity generation).

8. Create a single Cavity & Core Body to be split by the Parting Surfaces.

9. Create Bottom Half (Core Body) by trimming solid body using the Inside Parting Surface.

10. Create Top Half (Cavity Body) by trimming solid body using the Outside Parting Surface.

11. Create external Core and Cavity part files by "Associate BREP with body". Right click on the body for this option.

 

This is a very simple part in this example, but hopefully it is sufficient for you to understand the principle.

 

Malcolm

IRONCAD_2017_PU1.1___Sample_Mould_Cavity_and_Core_Generation___Steps.mp4

Hexagon_Part___Cavity_and_Core_Generation.ics

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Ya, as expected nothing is working. Your videos don't make sense. I cannot upload the files in the new 2017 version nor can I duplicate what's in the video? Lost absolutely lost! I can create simple structures and extract some surfaces. Trial and error more like years of trying and not figuring it out. I appreciate the effort trying to show me how to create a mold cavity, even after my 4 day training I cannot make anything work.

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Pitching in. The way I did it in the past is make sure the part that will form the a cavity of a mold is set 0,0,0 or as common term nest on the datum plane. On Menu>View>Toolbars>Customize>Toolbars tab, tick Boolean Operation

Toolbar.png

 

Select the model and click the first button of the Boolean Operation toolbar to set operation as a negative or positive object intellishape when you drag it to a mold block. Use the tri-ball to put it on place.

 

There was an old IRONCAD document which illustrate basic mold making capabilities. I have to look for it later.

 

 

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Ya, as expected nothing is working. Your videos don't make sense. I cannot upload the files in the new 2017 version nor can I duplicate what's in the video? Lost absolutely lost! I can create simple structures and extract some surfaces. Trial and error more like years of trying and not figuring it out. I appreciate the effort trying to show me how to create a mold cavity, even after my 4 day training I cannot make anything work.

46610[/snapback]

 

 

D

I will try to put some videos together for you. But in the meantime, if you have very complex parting lines, theres no simply split tool to achieve this in one function. I have to believe even in "high-end" systems" this is not a one click operation. Anyway, what I do is use the auto-feature selection filter to extract the inner surfaces to a new surface for the Core. On simply parts this works great and is a one click operation.

 

But I will review your entire post and see if I can come up with soemthing for you.

tom

 

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